Ansys 11 tutorial

1.ANSYS CFXTutorialsANSYS CFX Release 11.0December 20062. ANSYS, Inc.Southpointe275 Technology DriveCanonsburg, PA [email protected]://www.ansys.com(T) 724-746-3304(F) 724-514-94943. Copyright and Trademark Information© 1996-2006 ANSYS Europe, Ltd. All rights reserved. Unauthorized use, distribution, or duplication isprohibited. ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or itssubsidiaries located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service andfeature names or trademarks are the property of their respective owners. Disclaimer NoticeTHIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARECONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under asoftware license agreement that contains provisions concerning non-disclosure, copying, length andnature of use, compliance with exporting laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license agreement. ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001:2000 companies. U.S. Government RightsFor U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement,the use, duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software license agreement and FAR 12.212 (for non DOD licenses).Third-Party Software See the online documentation in the product help files for the complete Legal Notice for ANSYSproprietary software and third-party software. The ANSYS third-party software information is alsoavailable via download from the Customer Portal on the ANSYS web page. If you are unable to access thethird-party legal notices, please contact ANSYS, Inc.Published in the U.S.A.4. Table of ContentsCopyright and Trademark InformationDisclaimer NoticeU.S. Government RightsThird-Party SoftwareIntroduction to theANSYS CFX Tutorials Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Setting the Working Directory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Changing the Display Colors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2Tutorial 1:Simulating Flow in a Static Mixer Using CFX in Standalone Mode Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Tutorial 1 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .12 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .15Tutorial 1a:Simulating Flow in a Static Mixer Using Workbench Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31 Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32 Tutorial 1a Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32ANSYS CFX Tutorials Page v5. Table of Contents: Tutorial 2: Flow in a Static Mixer (Refined Mesh)Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .33Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .34Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .43Tutorial 2:Flow in a Static Mixer(Refined Mesh)Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .59Tutorial 2 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .60Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .60Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .61Obtaining a Solution Using Interpolation with ANSYS CFX-Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .66Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .68Tutorial 3:Flow in a Process Injection Mixing PipeIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .77Tutorial 3 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .78Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .78Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .79Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .87Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .88Tutorial 4:Flow from a Circular VentIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .93Tutorial 4 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .94Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .95Defining a Steady-State Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .95Obtaining a Solution to the Steady-State Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .99Defining a Transient Simulation in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100Obtaining a Solution to the Transient Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105Tutorial 5:Flow Around a Blunt BodyIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109Tutorial 5 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111Page viANSYS CFX Tutorials6. Table of Contents: Tutorial 6: Buoyant Flow in a Partitioned Cavity Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119Tutorial 6:Buoyant Flow in a Partitioned Cavity Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127 Tutorial 6 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135Tutorial 7:Free Surface Flow Over a Bump Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Tutorial 7 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149 Using a Supercritical Outlet Condition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154Tutorial 8:Supersonic Flow Over a Wing Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Tutorial 8 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162Tutorial 9:Flow Through a Butterfly Valve Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165 Tutorial 9 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180Tutorial 10:ANSYS CFX TutorialsPage vii7. Table of Contents: Tutorial 11: Non-Newtonian Fluid Flow in an AnnulusFlow in a Catalytic ConverterIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185Tutorial 10 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 193Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 194Tutorial 11:Non-Newtonian Fluid Flow in an AnnulusIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199Tutorial 11 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 200Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 201Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 201Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 205Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 206Tutorial 12:Flow in an Axial Rotor/StatorIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 207Tutorial 12 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 208Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 209Defining a Frozen Rotor Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 210Obtaining a Solution to the Frozen Rotor Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214Viewing the Frozen Rotor Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 215Setting up a Transient Rotor-Stator Calculation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 216Obtaining a Solution to the Transient Rotor-Stator Model. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220Tutorial 13:Reacting Flow in a Mixing TubeIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223Tutorial 13 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 224Outline of the Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 224Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 225Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237Tutorial 14:Page viiiANSYS CFX Tutorials8. Table of Contents: Tutorial 15: Multiphase Flow in Mixing VesselConjugate Heat Transfer in a Heating Coil Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239 Tutorial 14 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 240 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 246 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 246 Exporting the Results to ANSYS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247Tutorial 15:Multiphase Flow in Mixing Vessel Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251 Tutorial 15 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 252 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 265 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 265Tutorial 16:Gas-Liquid Flow in an Airlift Reactor Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269 Tutorial 16 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 270 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 270 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 277 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 278 Additional Fine Mesh Simulation Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 280Tutorial 17:Air Conditioning Simulation Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 283 Tutorial 17 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 295 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 295Tutorial 18:Combustion and Radiation in a Can Combustor Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 299ANSYS CFX Tutorials Page ix9. Table of Contents: Tutorial 19: Cavitation Around a HydrofoilTutorial 18 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 300Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301Using Eddy Dissipation and P1 Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 302Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308Laminar Flamelet and Discrete Transfer Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311Further Postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316Tutorial 19:Cavitation Around a HydrofoilIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317Tutorial 19 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 318Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319Creating an Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319Obtaining an Initial Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 323Viewing the Results of the Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324Preparing a Simulation with Cavitation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 326Obtaining a Cavitation Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328Viewing the Results of the Cavitation Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328Tutorial 20:Fluid Structure Interaction and Mesh DeformationIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 331Tutorial 20 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 332Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 333Using CEL Expressions to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334Using a Junction Box Routine to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343Tutorial 21:Oscillating Plate with Two-Way Fluid-Structure InteractionIntroduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 353Tutorial 21 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354Setting up the Solid Physics in Simulation (ANSYS Workbench) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 355Setting up the Fluid Physics and ANSYS Multi-field Settings in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . 358Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 364Viewing Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 365Tutorial 22:Page x ANSYS CFX Tutorials10. Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal CompressorOptimizing Flow in a Static Mixer Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 369 Tutorial 22 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 370 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 370 Creating the Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 371 Creating the Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 372 Creating the Mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 377 Overview of ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380 Setting the Output Parameter in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 386 Running Design Studies in DesignXplorer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 387Tutorial 23:Aerodynamic & Structural Performance of a Centrifugal Compressor Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 Tutorial 23 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 396 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 397 Reviewing the Centrifugal Compressor Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 397 Creating the Mesh in ANSYS TurboGrid . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 398 Defining the Aerodynamic Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 401 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 403 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 Importing Geometry into DesignModeler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405 Simulating Structural Stresses Due to Pressure Loads . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Simulating Structural Stresses Due to Rotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407ANSYS CFX Tutorials Page xi11. Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal CompressorPage xiiANSYS CFX Tutorials12. Introduction to theANSYS CFX TutorialsOverview These tutorials are designed to introduce general techniques used in ANSYS CFX and provide tips on advanced modeling. Earlier tutorials introduce general principles used in ANSYS CFX, including setting up the physical models, running ANSYS CFX-Solver and visualizing the results. The remaining tutorials highlight specialized features of ANSYS CFX. Files required to complete each tutorial is listed in the introduction to the tutorial, and located in /examples, where is the installation directory.Setting the Working Directory One of the first things you must do when using ANSYS CFX is to set a working directory. The working directory is the default location for loading and saving files for a particular session or project. The working directory is set according to how you run ANSYS CFX: • Workbench Set the working directory by saving a project file. • Standalone Set the working directory by entering it in CFX Launcher.ANSYS CFX Tutorials Page 1ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.13. Introduction to the ANSYS CFX Tutorials: Changing the Display ColorsChanging the Display ColorsIf viewing objects in ANSYS CFX becomes difficult due to contrast with the background, thecolors can be altered for improved viewing. The color options are set in different places,depending on how you run ANSYS CFX, as follows:• In standalone mode (i.e., after using CFX Launcher to launch ANSYS CFX-Pre or ANSYSCFX-Post):a. Select Edit > Options. The Options dialog box appears.b. Adjust the color settings under CFX-Pre > Viewer (for ANSYS CFX-Pre) or CFX-Post > Viewer (for ANSYS CFX-Post).c. Click OK.• In ANSYS Workbench:a. Select Tools > Options from the Project page.b. Adjust the color settings under Common Settings > Graphics Style.c. Click OK.Page 2 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.14. Tutorial 1:Simulating Flow in a StaticMixer Using CFX in StandaloneModeIntroduction This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. This tutorial includes: • Before You Begin (p. 4) • Tutorial 1 Features (p. 4) • Overview of the Problem to Solve (p. 5) • Defining a Simulation in ANSYS CFX-Pre (p. 6) • Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12) • Viewing the Results in ANSYS CFX-Post (p. 15) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) To learn how to perform these tasks in Workbench, see Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench (p. 31 in "ANSYS CFX Tutorials").ANSYS CFX Tutorials Page 3ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.15. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Before You BeginBefore You BeginCreate a working directory for your files. Once this is done, copy the sample files used in thistutorial to your working directory from the installation folder for your software(/examples/ (for example, C:Program FilesANSYSIncv110CFXexamples)) to avoid overwriting source files provided with yourinstallation. If you plan to use a session file, please refer to Playing a Session File (p. 7).Sample files used by this tutorial are:• StaticMixerMesh.gtm• StaticMixer.preTutorial 1 FeaturesThis tutorial addresses the following features of ANSYS CFX. Component FeatureDetails ANSYS CFX-Pre User ModeQuick Setup Wizard Simulation TypeSteady State Fluid Type General Fluid Domain TypeSingle Domain Turbulence Model k-Epsilon Heat TransferThermal Energy Boundary ConditionsInlet (Subsonic)Outlet (Subsonic)Wall: No-SlipWall: Adiabatic Timestep Physical Time Scale ANSYS CFX-PostPlotsAnimationContourOutline Plot (Wireframe)PointSlice PlaneStreamlineIn this tutorial you will learn about:• Using Quick Setup mode in ANSYS CFX-Pre to set up a problem.• Modifying the outline plot in ANSYS CFX-Post.• Using streamlines in ANSYS CFX-Post to trace the flow field from a point.• Viewing temperature using colored planes and contours in ANSYS CFX-Post.• Creating an animation and saving it to an MPEG file.Page 4 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.16. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Overview of the Problem to SolveOverview of the Problem to Solve This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. Water enters through both pipes at the same rate but at different temperatures. The first entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2 m/s at a temperature of 285 K. The radius of the mixer is 2 m. Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and temperature of the water when it exits the static mixer. Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe 2 m/sr=2m 285 K2 m/s315 KANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 5Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.17. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-PreDefining a Simulation in ANSYS CFX-PreBecause you are starting with an existing mesh, you can immediately use ANSYS CFX-Pre todefine the simulation. This is how ANSYS CFX-Pre will look with the imported mesh:In the image above, the left pane of ANSYS CFX-Pre displays the Outline . When youdouble-click on items in the Outline, the Outline editor opens and can be used to create,modify, and view objects.Note: In this documentation, the details view can also be referenced by the name of theobject being edited, followed by the word “details view” (for example, if you double-clickthe Wireframe object, the Wireframe details view appears).Synopsis of Quick Setup ModeQuick Setup mode provides a simple wizard–like interface for setting up simple cases. Thisis useful for getting familiar with the basic elements of a CFD problem setup. This sectiondescribes using Quick Setup mode to develop a simulation in ANSYS CFX-Pre.Workflow OverviewThis tutorial follows the general workflow for Quick Setup mode:1. Creating a New Simulation (p. 7)2. Setting the Physics Definition (p. 7)3. Importing a Mesh (p. 7)4. Defining Model Data (p. 9)5. Defining Boundaries (p. 9)Page 6 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.18. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre 6. Setting Boundary Data (p. 9) 7. Setting Flow Specification (p. 9) 8. Setting Temperature Specification (p. 10) 9. Reviewing the Boundary Condition Definitions (p. 10) 10. Creating the Second Inlet Boundary Definition (p. 10) 11. Creating the Outlet Boundary Definition (p. 10) 12. Moving to General Mode (p. 11) 13. Writing the Solver (.def) File (p. 11)Playing aIf you want to skip past these instructions and have ANSYS CFX-Pre set up the simulationSession File automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 12). After you have played the session file, proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).Creating a New Simulation Before importing and working with a mesh, a simulation needs to be started using Quick Setup mode.Procedure1. If required, launch ANSYS CFX-Pre. 2. Select File > New Simulation.The New Simulation File dialog box is displayed. 3. Select Quick Setup and click OK. Note: If this is the first time you are running this software, a message box will appear notifying you that automatic generation of the default domain is active. To avoid seeing this message again uncheck Show This Message Again. 4. Select File > Save Simulation As. 5. Under File name, type: StaticMixer 6. Click Save.Setting the Physics Definition You need to specify the fluids used in a simulation. A variety of fluids are already defined as library materials. For this tutorial you will use a prepared fluid, Water, which is defined to be water at 25°C.Procedure1. Ensure that Simulation Definition is displayed at the top of the details view. 2. Under Fluid select Water.Importing a Mesh At least one mesh must be imported before physics are applied.Procedure1. In Simulation Definition, under Mesh File, click Browse . The Import Mesh dialog box appears.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 7Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.19. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre2. Under File type, select CFX Mesh (*gtm *cfx).3. From your working directory, select StaticMixerMesh.gtm.4. Click Open. The mesh loads.5. Click Next.Using the ViewerNow that the mesh is loaded, take a moment to explore how you can use the viewer toolbarto zoom in or out and to rotate the object in the viewer.Using the ZoomThere are several icons available for controlling the level of zoom in the viewer.Tools1. Click Zoom Box2. Click and drag a rectangular box over the geometry.3. Release the mouse button to zoom in on the selection. The geometry zoom changes to display the selection at a greater resolution.4. Click Fit View to re-center and re-scale the geometry.Rotating theIf you need to rotate an object or to view it from a new angle, you can use the viewer toolbar.geometry1. Click Rotateon the viewer toolbar.2. Click and drag within the geometry repeatedly to test the rotation of the geometry. The geometry rotates based on the direction of movement. Notice how the mouse cursor changes depending on where you are in the viewer:3. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X).4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z Up).A clearer view of the mesh is displayed.Page 8 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.20. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-PreDefining Model Data You need to define the type of flow and the physical models to use in the fluid domain. You will specify the flow as steady state with turbulence and heat transfer. Turbulence is modeled using the k - ε turbulence model and heat transfer using the thermal energy model. The k - ε turbulence model is a commonly used model and is suitable for a wide range of applications. The thermal energy model neglects high speed energy effects and is therefore suitable for low speed flow applications.Procedure1. Ensure that Physics Definition is displayed. 2. Under Model Data, set Reference Pressure to 1 [atm].All other pressure settings are relative to this reference pressure. 3. Set Heat Transfer to Thermal Energy. 4. Set Turbulence to k-Epsilon. 5. Click Next.Defining Boundaries The CFD model requires the definition of conditions on the boundaries of the domain.Procedure1. Ensure that Boundary Definition is displayed. 2. Delete Inlet and Outlet from the list by right-clicking each and selecting Delete. 3. Right-click in the blank area where Inlet and Outlet were listed, then select New. 4. Set Name to in1. 5. Click OK. The boundary is created and, when selected, properties related to the boundary are displayed.Setting Boundary Data Once boundaries are created, you need to create associated data. Based on Figure 1, you will define the first inlet boundary condition’s velocity and temperature.Procedure1. Ensure that Boundary Data is displayed. 2. Set Boundary Type to Inlet. 3. Set Location to in1.Setting Flow Specification Once boundary data is defined, the boundary needs to have the flow specification assigned.Procedure1. Ensure that Flow Specification is displayed. 2. Set Option to Normal Speed. 3. Set Normal Speed to 2 [m s^-1].ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 9Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.21. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-PreSetting Temperature SpecificationOnce flow specification is defined, the boundary needs to have temperature assigned.Procedure 1. Ensure that Temperature Specification is displayed.2. Set Static Temperature to 315 [K].Reviewing the Boundary Condition DefinitionsDefining the boundary condition for in1 required several steps. Here the settings arereviewed for accuracy.Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and atemperature of 315 K at one of the side inlets.Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows:Tab SettingValueBoundary Data Boundary TypeInletLocation in1Flow SpecificationOption Normal SpeedNormal Speed 2 [m s^-1]Temperature Specification Static Temperature 315 [K]Creating the Second Inlet Boundary DefinitionBased on Figure 1, you know the second inlet boundary condition consists of a velocity of 2m/s and a temperature of 285 K at one of the side inlets. You will define that now.Procedure 1. Under Boundary Definition, right-click in the selector area and select New.2. Create a new boundary named in2 with these settings:Tab SettingValueBoundary Data Boundary TypeInletLocation in2Flow SpecificationOption Normal SpeedNormal Speed 2 [m s^-1]Temperature Specification Static Temperature 285 [K]Creating the Outlet Boundary DefinitionNow that the second inlet boundary has been created, the same concepts can be applied tobuilding the outlet boundary.1. Create a new boundary named out with these settings:Page 10ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.22. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBoundary Data Boundary Type OutletLocationoutFlow SpecificationOptionAverage Static PressureRelative Pressure 0 [Pa] 2. Click Next.Moving to General Mode There are no further boundary conditions that need to be set. All 2D exterior regions that have not been assigned to a boundary condition are automatically assigned to the default boundary condition.Procedure1. Set Operation to Enter General Mode and click Finish. The three boundary conditions are displayed in the viewer as sets of arrows at the boundary surfaces. Inlet boundary arrows are directed into the domain. Outlet boundary arrows are directed out of the domain.Setting Solver Control Solver Control parameters control aspects of the numerical solution generation process. While an upwind advection scheme is less accurate than other advection schemes, it is also more robust. This advection scheme is suitable for obtaining an initial set of results, but in general should not be used to obtain final accurate results. The time scale can be calculated automatically by the solver or set manually. The Automatic option tends to be conservative, leading to reliable, but often slow, convergence. It is often possible to accelerate convergence by applying a time scale factor or by choosing a manual value that is more aggressive than the Automatic option. In this tutorial, you will select a physical time scale, leading to convergence that is twice as fast as the Automatic option.Procedure1. Click Solver Control . 2. On the Basic Settings tab, set Advection Scheme > Option to Upwind. 3. Set Convergence Control > Fluid Timescale Control > Timescale Control toPhysical Timescale and set the physical timescale value to 2 [s]. 4. Click OK.Writing the Solver (.def) File The simulation file, StaticMixer.cfx, contains the simulation definition in a format that can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and modify the simulation definition. The simulation file differs from the definition file in that it can be saved at any time while defining the simulation.Procedure1. Click Write Solver File.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 11Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.23. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS The Write Solver File dialog box is displayed. 2. Set File name to StaticMixer.def. 3. Ensure that Start Solver Manager is selected from the drop down menu located inthe top-right corner of the dialog box. 4. Select Quit ANSYS CFX-Pre.This forces standalone ANSYS CFX-Pre to close after the definition file has been written. 5. Click Save. 6. If you are notified the file already exists, click Overwrite.This file is provided in the tutorial directory and may exist in your tutorial folder if youhave copied it there. 7. If prompted, click Yes or Save & Quit to save StaticMixer.cfx.The definition file (StaticMixer.def) and the simulation file (StaticMixer.cfx) arecreated. ANSYS CFX-Solver Manager automatically starts and the definition file is set inthe Define Run dialog box. 8. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).Playing the Session File and Starting ANSYS CFX-Solver Manager Note: This task is required only if you are starting here with the session file that was provided in the examples directory. If you have performed all the tasks in the previous steps, proceed directly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12). Events in ANSYS CFX-Pre can be recorded to a session file and then played back at a later date to drive ANSYS CFX-Pre. Session files have been created for each tutorial so that the problems can be set up rapidly in ANSYS CFX-Pre, if desired.Procedure1. If required, launch ANSYS CFX-Pre. 2. Select Session > Play Tutorial. 3. Select StaticMixer.pre. 4. Click Open.A definition file is written. 5. Select File > Quit. 6. Launch the ANSYS CFX-Solver Manager from CFX Launcher. 7. After the ANSYS CFX-Solver starts, select File > Define Run. 8. Under Definition File, click Browse . 9. Select StaticMixer.def, located in the working directory. 10. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12).Obtaining a Solution Using ANSYS CFX-Solver Manager ANSYS CFX-Solver Manager has a visual interface that displays a variety of results and should be used when plotted data needs to be viewed during problem solving.Page 12 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.24. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS Two windows are displayed when ANSYS CFX-Solver Manager runs. There is an adjustable split between the windows, which is oriented either horizontally or vertically depending on the aspect ratio of the entire ANSYS CFX-Solver Manager window (also adjustable). One window shows the convergence history plots and the other displays text output from ANSYS CFX-Solver. The text lists physical properties, boundary conditions and various other parameters used or calculated in creating the model. All the text is written to the output file automatically (in this case, StaticMixer_001.out).Start the Run The Define Run dialog box allows configuration of a run for processing by ANSYS CFX-Solver. When ANSYS CFX-Solver Manager is launched automatically from ANSYS CFX-Pre, all of the information required to perform a new serial run (on a single processor) is entered automatically. You do not need to alter the information in the Define Run dialog box. This is a very quick way to launch into ANSYS CFX-Solver without having to define settings and values.Procedure1. Ensure that the Define Run dialog box is displayed. 2. Click Start Run.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 13Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.25. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS ANSYS CFX-Solver launches and a split screen appears and displays the results of the run graphically and as text. The panes continue to build as ANSYS CFX-Solver Manager operates. Note: Once the second iteration appears, data begins to plot. Plotting may take a long time depending on the amount of data to process. Let the process run.Move from ANSYS CFX-Solver to ANSYS CFX-Post Once ANSYS CFX-Solver has finished, you can use ANSYS CFX-Post to review the finished results.Procedure1. When ANSYS CFX-Solver is finished, click Yes to post-process the results. After a short pause, ANSYS CFX-Post starts and ANSYS CFX-Solver Manager closes.Page 14 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.26. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostViewing the Results in ANSYS CFX-Post When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed. The viewer displays an outline of the geometry and other graphic objects. You can use the mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre.Workflow Overview This tutorial describes the following workflow for viewing results in ANSYS CFX-Post: 1. Setting the Edge Angle for a Wireframe Object (p. 16) 2. Creating a Point for the Origin of the Streamline (p. 17) 3. Creating a Streamline Originating from a Point (p. 18) 4. Rearranging the Point (p. 19) 5. Configuring a Default Legend (p. 19) 6. Creating a Slice Plane (p. 20) 7. Defining Slice Plane Geometry (p. 21) 8. Configuring Slice Plane Views (p. 21) 9. Rendering Slice Planes (p. 22) 10. Coloring the Slice Plane (p. 23) 11. Moving the Slice Plane (p. 23) 12. Adding Contours (p. 24) 13. Working with Animations (p. 25) 14. Showing the Animation Dialog Box (p. 25)ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 15Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.27. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post15. Creating the First Keyframe (p. 26)16. Creating the Second Keyframe (p. 26)17. Viewing the Animation (p. 27)18. Modifying the Animation (p. 28)19. Saving to MPEG (p. 29)Setting the Edge Angle for a Wireframe ObjectThe outline of the geometry is called the wireframe or outline plot.By default, ANSYS CFX-Post displays only some of the surface mesh. This sometimes meansthat when you first load your results file, the geometry outline is not displayed clearly. Youcan control the amount of the surface mesh shown by editing the Wireframe object listedin the Outline.The check boxes next to each object name in the Outline control the visibility of eachobject. Currently only the Wireframe and Default Legend objects have visibility selected.The edge angle determines how much of the surface mesh is visible. If the angle betweentwo adjacent faces is greater than the edge angle, then that edge is drawn. If the edge angleis set to 0°, the entire surface mesh is drawn. If the edge angle is large, then only the mostsignificant corner edges of the geometry are drawn.For this geometry, a setting of approximately 15° lets you view the model location withoutdisplaying an excessive amount of the surface mesh.In this module you can also modify the zoom settings and view of the wireframe.Procedure 1. In the Outline, under User Locations and Plots, double-click Wireframe.Tip: While it is not necessary to change the view to set the angle, do so to explore thepractical uses of this feature.2. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select Isometric View (Z up).3. In the Wireframe details view, under Definition, click in the Edge Angle box. An embedded slider is displayed.4. Type a value of 10 [degree].5. Click Apply to update the object with the new setting.Page 16ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.28. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Notice that more surface mesh is displayed. 6. Drag the embedded slider to set the Edge Angle value to approximately 45 [degree]. 7. Click Apply to update the object with the new setting.Less of the outline of the geometry is displayed. 8. Type a value of 15 [degree]. 9. Click Apply to update the object with the new setting. 10. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select View Towards -X.Creating a Point for the Origin of the Streamline A streamline is the path that a particle of zero mass would follow through the domain.Procedure1. Select Insert > Location > Point from the main menu.You can also use the toolbars to create a variety of objects. Later modules and tutorialsexplore this further. 2. Click OK.This accepts the default name. 3. Under Definition, ensure that Method is set to XYZ. 4. Under Point, enter the following coordinates: -1, -1, 1.This is a point near the first inlet. 5. Click Apply. The point appears as a symbol in the viewer as a crosshair symbol.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 17Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.29. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostCreating a Streamline Originating from a PointWhere applicable, streamlines can trace the flow direction forwards (downstream) and/orbackwards (upstream).Procedure 1. From the main menu, select Insert > Streamline. You can also use the toolbars to create a variety of objects. Later modules and tutorials will explore this further.2. Click OK. This accepts the default name.3. Under Definition, in Start From, ensure that Point 1 is set.Tip: To create streamlines originating from more than one location, click the ellipsis iconto the right of the Start From box. This displays the Location Selector dialog box,where you can use the and keys to pick multiple locators.4. Click the Color tab.5. Set Mode to Variable.6. Set Variable to Total Temperature.7. Set Range to Local.8. Click Apply. The streamline shows the path of a zero mass particle from Point 1. The temperature is initially high near the hot inlet, but as the fluid mixes the temperature drops.Page 18ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.30. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostRearranging the Point Once created, a point can be rearranged manually or by setting specific coordinates. Tip: In this module, you may choose to display various views and zooms from the Predefined Camera option in the shortcut menu (such as Isometric View (Z up) or View Towards -X) and by using Zoom Box if you prefer to change the display.Procedure1. In Outline, under User Locations and Plots double-click Point 1.Properties for the selected user location are displayed. 2. Under Point, set these coordinates: -1, -2.9, 1. 3. Click Apply.The point is moved and the streamline redrawn. 4. In the selection tools, click Single Select. While in this mode, the normal behavior of the left mouse button is disabled. 5. In the viewer, drag Point 1 (appears as a yellow addition sign) to a new location withinthe mixer.The point position is updated in the details view and the streamline is redrawn at thenew location. The point moves normal in relation to the viewing direction. 6. Click Rotate. Tip: You can also click in the viewer area, and press the space bar to toggle between Select and Viewing Mode. A way to pick objects from Viewing Mode is to hold down + while clicking on an object with the left mouse button. 7. Under Point, reset these coordinates: -1, -1, 1. 8. Click Apply.The point appears at its original location. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X.Configuring a Default Legend You can modify the appearance of the default legend. The default legend appears whenever a plot is created that is colored by a variable. The streamline color is based on temperature; therefore, the legend shows the temperature range. The color pattern on the legend’s color bar is banded in accordance with the bands in the plot1. 1. An exception occurs when one or more bands in a contour plot represent values beyond thelegend’s range. In this case, such bands are colored using a color that is extrapolated slightlypast the range of colors shown in the legend. This can happen only when a user-specifiedrange is used for the legend.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 19Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.31. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostThe default legend displays values for the last eligible plot that was opened in the detailsview. To maintain a legend definition during an ANSYS CFX-Post session, you can create anew legend by clicking Legend .Because there are many settings that can be customized for the legend, this module allowsyou the freedom to experiment with them. In the last steps you will set up a legend, basedon the default legend, with a minor modification to the position.Tip: When editing values, you can restore the values that were present when you beganediting by clicking Reset. To restore the factory-default values, click Default.Procedure 1. Double click Default Legend View 1. The Definition tab of the default legend is displayed.2. Apply the following settingsTabSetting ValueDefinition Title ModeUser Specified Title Streamline Temp. Horizontal(Selected) Location > Y JustificationBottom3. Click Apply. The appearance and position of the legend changes based on the settings specified.4. Modify various settings in Definition and click Apply after each change.5. Select Appearance.6. Modify a variety of settings in the Appearance and click Apply after each change.7. Click Defaults.8. Click Apply.9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and Streamline 1.Since both are no longer visible, the associated legend no longer appears.Creating a Slice PlaneDefining a slice plane allows you to obtain a cross–section of the geometry.In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic objectcould be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed coloror it can vary based on the value of a variable.You already have some objects defined by default (listed in the Outline). You can viewresults on the boundaries of the static mixer by coloring each boundary object by a variable.To view results within the geometry (that is, on non-default locators), you will create newobjects.You can use the following methods to define a plane:• Three Points: creates a plane from three specified points.Page 20ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.32. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post • Point and Normal: defines a plane from one point on the plane and a normal vector to the plane. • YZ Plane, ZX Plane, and XY Plane: similar to Point and Normal, except that the normal is defined to be normal to the indicated plane.Procedure1. From the main menu, select Insert > Location > Plane or click Location > Plane. 2. In the New Plane window, type: Slice 3. Click OK.The Geometry, Color, Render and View tabs let you switch between settings. 4. Click the Geometry tab.Defining Slice Plane Geometry You need to choose the vector normal to the plane. You want the plane to lie in the x-y plane, hence its normal vector points along the z-axis. You can specify any vector that points in the z-direction, but you will choose the most obvious (0,0,1).Procedure1. If required, under Geometry, expand Definition. 2. Under Method select Point and Normal. 3. Under Point enter 0,0,1. 4. Under Normal enter 0, 0,1. 5. Click Apply. Slice appears under User Locations and Plots. Rotate the view to see the plane.Configuring Slice Plane Views Depending on the view of the geometry, various objects may not appear because they fall in a 2D space that cannot be seen.Procedure1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z up).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 21Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.33. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostThe slice is now visible in the viewer.2. Click Zoom Box.3. Click and drag a rectangular selection over the geometry.4. Release the mouse button to zoom in on the selection.5. Click Rotate .6. Click and drag the mouse pointer down slightly to rotate the geometry towards you.7. Select Isometric View (Z up) as described earlier.Rendering Slice PlanesRender settings determine how the plane is drawn.Procedure 1. Select the Render tab.2. Clear Draw Faces.3. Select Draw Lines.4. Under Draw Lines change Color Mode to User Specified.5. Click the current color in Line Color to change to a different color. For a greater selection of colors, click the ellipsis to use the Select color dialog box.6. Click Apply.7. Click Zoom Box.8. Zoom in on the geometry to view it in greater detail.Page 22ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.34. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post The line segments show where the slice plane intersects with mesh element faces. The end points of each line segment are located where the plane intersects mesh element edges. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z.The image shown below can be used for comparison with tutorial 2 (in the sectionCreating a Slice Plane (p. 68)), where a refined mesh is used.Coloring the Slice Plane The Color panel is used to determine how the object faces are colored.Procedure1. Apply the following settings to SliceTab Setting ValueColor ModeVariable*VariableTemperatureRenderDraw Faces(Selected)Draw Lines(Cleared) *.You can specify the variable (in this case, temperature) used to color the graphic element. The Constant mode allows you to color the plane with a fixed color. 2. Click Apply. Hot water (red) enters from one inlet and cold water (blue) from the other.Moving the Slice Plane The plane can be moved to different locations.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 23Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.35. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostProcedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.2. Click the Geometry tab. Review the settings in Definition under Point and under Normal.3. Click Single Select .4. Click and drag the plane to a new location that intersects the domain. As you drag the mouse, the viewer updates automatically. Note that Point updates with new settings.5. Set Point settings to 0,0,1.6. Click Apply.7. Click Rotate .8. Turn off visibility for Slice by clearing the check box next to Slice in the Outline.Adding ContoursContours connect all points of equal value for a scalar variable (for example, Temperature)and help to visualize variable values and gradients. Colored bands fill the spaces betweencontour lines. Each band is colored by the average color of its two bounding contour lines(even if the latter are not displayed).Procedure 1. Select Insert > Contour from the main menu or click Contour.The New Contour dialog box is displayed.2. Set Name to Slice Contour.3. Click OK.4. Apply the following settingsTabSetting ValueGeometry Locations Slice VariableTemperatureRender Draw Faces(Selected)5. Click Apply.Important: The colors of 3D graphics object faces are slightly altered when lighting is on. Toview colors with highest accuracy, clear Lighting under Draw Faces on the Render tab andclick Apply.Page 24ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.36. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post The graphic element faces are visible, producing a contour plot as shown. Note: Make sure that the checkbox next to Slice in the Outline is cleared.Working with Animations Animations build transitions between views for development of video files.Workflow This tutorial follows the general workflow for creating a keyframe animation:Overview 1. Showing the Animation Dialog Box (p. 25) 2. Creating the First Keyframe (p. 26) 3. Creating the Second Keyframe (p. 26) 4. Viewing the Animation (p. 27) 5. Modifying the Animation (p. 28) 6. Saving to MPEG (p. 29)Showing the Animation Dialog Box The Animation dialog box is used to define keyframes and to export to a video file.Procedure1. Select Tools > Animation or click Animation . The Animation dialog box can be repositioned as required.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 25Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.37. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostCreating the First KeyframeKeyframes are required in order to produce an animation. You need to define the first viewerstate, a second (and final) viewer state, and set the number of interpolated intermediateframes.Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).2. In the Outline, under User Locations and Plots, clear the visibility of Slice Contour and select the visibility of Slice.3. In the Animation dialog box, click New.A new keyframe named KeyframeNo1 is created. This represents the current imagedisplayed in the viewer.Creating the Second KeyframeKeyframes are required in order to produce an animation.Procedure 1. In the Outline, under User Locations and Plots, double-click Slice.2. On the Geometry tab, set Point coordinate values to (0,0,-1.99).3. Click Apply. The slice plane moves to the bottom of the mixer.4. In the Animation dialog box, click New.KeyframeNo2 is created and represents the image displayed in the Viewer.Page 26ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.38. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post 5. Select KeyframeNo1. 6. Set # of Frames (located below the list of keyframes) to 20.This is the number of intermediate frames used when going from KeyframeNo1 toKeyframeNo2. This number is displayed in the Frames column for KeyframeNo1. 7. Press Enter.The Frame # column shows the frame in which each keyframe appears. KeyframeNo1appears at frame 1 since it defines the start of the animation. KeyframeNo2 is at frame22 since you have 20 intermediate frames (frames 2 to 21) in between KeyframeNo1 andKeyframeNo2.Viewing the Animation More keyframes could be added, but this animation has only two keyframes (which is the minimum possible).Synopsis The controls previously greyed-out in the Animation dialog box are now available. The number of intermediate frames between keyframes is listed beside the keyframe having the lowest number of the pair. The number of keyframes listed beside the last keyframe is ignored.Procedure1. Click Play the animation. The animation plays from frame 1 to frame 22. It plays relatively slowly because the slice plane must be updated for each frame.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 27Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.39. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostModifying the AnimationTo make the plane sweep through the whole geometry, you will set the starting position ofthe plane to be at the top of the mixer. You will also modify the Range properties of theplane so that it shows the temperature variation better. As the animation is played, you cansee the hot and cold water entering the mixer. Near the bottom of the mixer (where thewater flows out) you can see that the temperature is quite uniform. The new temperaturerange lets you view the mixing process more accurately than the global range used in thefirst animation.Procedure 1. Apply the following settings to SliceTab SettingValueGeometryPoint0, 0, 1.99Color Variable TemperatureRangeUser SpecifiedMin295 [K]Max305 [K]2. Click Apply. The slice plane moves to the top of the static mixer.Note: Do not double click in the next step.3. In the Animation dialog box, single click (do not double-click) KeyframeNo1 to select it. If you had double-clicked KeyFrameNo1, the plane and viewer states would have been redefined according to the stored settings for KeyFrameNo1. If this happens, clickUndo and try again to select the keyframe.4. Click Set Keyframe .The image in the Viewer replaces the one previously associated with KeyframeNo1.5. Double-click KeyframeNo2. The object properties for the slice plane are updated according to the settings in KeyFrameNo2.6. Apply the following settings to SliceTab SettingValueColor Variable TemperatureRangeUser SpecifiedMin295 [K]Max305 [K]7. Click Apply.8. In the Animation dialog box, single-click KeyframeNo2.9. Click Set Keyframe to save the new settings to KeyframeNo2.Page 28ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.40. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostSaving to MPEG By defining the geometry and then saving to MPEG, the results can be saved to a video file.Procedure1. Click More Animation Options to view the additional options. The Loop and Bounce radio buttons determine what happens when the animation reaches the last keyframe. When Loop is selected, the animation repeats itself the number of times defined by Repeat. When Bounce is selected, every other cycle is played in reverse order, starting with the second. 2. Click Save MPEG. 3. Click Browsenext to Save MPEG. 4. Under File name type: StaticMixer.mpg 5. If required, set the path location to a different folder. 6. Click Save.The MPEG file name (including path) is set. At this point, the animation has not yet beenproduced. 7. Click Previous Keyframe .Wait a moment as the display updates the keyframe display. 8. Click Play the animation. 9. If prompted to overwrite an existing movie click Overwrite.The animation plays and builds an MPEG file. 10. Click the Options button at the bottom of the Animation dialog box. In Advanced, you can see that a Frame Rate of 24 frames per second was used to create the animation. The animation you produced contains a total of 22 frames, so it takes just under 1 second to play in a media player. 11. Click Cancel to close the dialog box. 12. Close the Animation dialog box. 13. Review the animation in third–party software as required.Exiting ANSYS CFX-Post When finished with ANSYS CFX-Post exit the current window: 1. When you are finished, select File > Quit to exit ANSYS CFX-Post. 2. Click Quit if prompted to save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 29Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.41. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-PostPage 30ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.42. Tutorial 1a:Simulating Flow in a StaticMixer Using WorkbenchIntroduction This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. This tutorial comprises: • Before You Begin (p. 32) • Tutorial 1a Features (p. 32) • Overview of the Problem to Solve (p. 33) • Defining a Simulation in ANSYS CFX-Pre (p. 34) • Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41) • Viewing the Results in ANSYS CFX-Post (p. 43) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) To learn how to perform these tasks using CFX in Standalone mode, see Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3 in "ANSYS CFX Tutorials").ANSYS CFX TutorialsPage 31ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.43. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Before You BeginBefore You BeginCreate a working directory for your files. Once this is done, copy the sample files used in thistutorial to your working directory from the installation folder for your software(/examples/ (for example, C:Program FilesANSYSIncv110CFXexamples)) to avoid overwriting source files provided with yourinstallation. If you plan to use a session file, please refer to Playing a Session File (p. 35).Sample files used by this tutorial are:• StaticMixerMesh.gtm• StaticMixer.preTutorial 1a FeaturesThis tutorial addresses the following features of ANSYS CFX. Component FeatureDetails ANSYS CFX-Pre User ModeQuick Setup Wizard Simulation TypeSteady State Fluid Type General Fluid Domain TypeSingle Domain Turbulence Model k-Epsilon Heat TransferThermal Energy Boundary ConditionsInlet (Subsonic)Outlet (Subsonic)Wall: No-SlipWall: Adiabatic Timestep Physical Time Scale ANSYS CFX-PostPlotsAnimationContourOutline Plot (Wireframe)PointSlice PlaneStreamlineIn this tutorial you will learn about:• Using Quick Setup mode in ANSYS CFX-Pre to set up a problem.• Modifying the outline plot in ANSYS CFX-Post.• Using streamlines in ANSYS CFX-Post to trace the flow field from a point.• Viewing temperature using colored planes and contours in ANSYS CFX-Post.• Creating an animation and saving it to an MPEG file.Page 32ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.44. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Overview of the Problem to SolveOverview of the Problem to Solve This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. Water enters through both pipes at the same rate but at different temperatures. The first entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2 m/s at a temperature of 285 K. The radius of the mixer is 2 m. Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and temperature of the water when it exits the static mixer. Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe 2 m/sr=2m 285 K2 m/s315 KANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 33Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.45. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-PreDefining a Simulation in ANSYS CFX-PreBecause you are starting with an existing mesh, you can immediately use ANSYS CFX-Pre todefine the simulation. This is how ANSYS CFX-Pre will look with the imported mesh:In the image above, the left pane of ANSYS CFX-Pre displays the Outline. When youdouble-click on items in the Outline, the Outline editor opens and can be used to create,modify, and view objects.Note: In this documentation, the details view can also be referenced by the name of theobject being edited, followed by the word “details view” (for example, if you double-clickthe Wireframe object, the Wireframe details view appears).Synopsis of Quick Setup ModeQuick Setup mode provides a simple wizard–like interface for setting up simple cases. Thisis useful for getting familiar with the basic elements of a CFD problem setup. This sectiondescribes using Quick Setup mode to develop a simulation in ANSYS CFX-Pre.Workflow OverviewThis tutorial follows the general workflow for Quick Setup mode:1. Creating a New Simulation (p. 35)2. Setting the Physics Definition (p. 35)3. Importing a Mesh (p. 36)4. Defining Model Data (p. 37)5. Defining Boundaries (p. 37)Page 34ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.46. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre 6. Setting Boundary Data (p. 37) 7. Setting Flow Specification (p. 37) 8. Setting Temperature Specification (p. 38) 9. Reviewing the Boundary Condition Definitions (p. 38) 10. Creating the Second Inlet Boundary Definition (p. 38) 11. Creating the Outlet Boundary Definition (p. 39) 12. Moving to General Mode (p. 39) 13. Writing the Solver (.def) File (p. 40)Playing aIf you want to skip past these instructions and have ANSYS CFX-Pre set up the simulationSession File automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 40). After you have played the session file, proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41).Creating a New Simulation Before importing and working with a mesh, a simulation needs to be started using Quick Setup mode.Procedure1. If required, launch ANSYS Workbench. 2. Click Empty Project.The Project page appears displaying an unsaved project. 3. Select File > Save or click Save . 4. If required, set the path location to the working folder you created for this tutorial. 5. Under File name, type: StaticMixer 6. Click Save. 7. On the left-hand task bar under Advanced CFD, click Start CFX-Pre. 8. Select File > New Simulation. 9. Select Quick Setup in the New Simulation File dialog box and click OK. 10. Select File > Save Simulation As. 11. Under File name, type: StaticMixer 12. Click Save.Setting the Physics Definition You need to specify the fluids used in a simulation. A variety of fluids are already defined as library materials. For this tutorial you will use a prepared fluid, Water, which is defined to be water at 25°C.Procedure1. Ensure that Simulation Definition is displayed at the top of the Details view. 2. Under Fluid select Water.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 35Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.47. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-PreImporting a MeshAt least one mesh must be imported before physics are applied.Procedure 1. In Simulation Definition, under Mesh File, click Browse .The Import Mesh dialog box appears.2. Under File type, select CFX Mesh (*gtm).3. From your working directory, select StaticMixerMesh.gtm.4. Click Open. The mesh loads.5. Click Next.Using the ViewerNow that the mesh is loaded, take a moment to explore how you can use the viewer toolbarto zoom in or out and to rotate the object in the viewer.Using the ZoomThere are several icons available for controlling the level of zoom in the viewer.Tools1. Click Zoom Box2. Click and drag a rectangular box over the geometry.3. Release the mouse button to zoom in on the selection. The geometry zoom changes to display the selection at a greater resolution.4. Click Fit View to re-center and re-scale the geometry.Rotating theIf you need to rotate an object or to view it from a new angle, you can use the viewer toolbar.geometry1. Click Rotateon the viewer toolbar.2. Click and drag within the geometry repeatedly to test the rotation of the geometry. The geometry rotates based on the direction of movement. Notice how the mouse cursor changes depending on where you are in the viewer:3. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X).Page 36ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.48. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre 4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z Up). A clearer view of the mesh is displayed.Defining Model Data You need to define the type of flow and the physical models to use in the fluid domain. You will specify the flow as steady state with turbulence and heat transfer. Turbulence is modelled using the k - ε turbulence model and heat transfer using the thermal energy model. The k - ε turbulence model is a commonly used model and is suitable for a wide range of applications. The thermal energy model neglects high speed energy effects and is therefore suitable for low speed flow applications.Procedure1. Ensure that Physics Definition is displayed. 2. Under Model Data, set Reference Pressure to 1 [atm].All other pressure settings are relative to this reference pressure. 3. Set Heat Transfer to Thermal Energy. 4. Set Turbulence to k-Epsilon. 5. Click Next.Defining Boundaries The CFD model requires the definition of conditions on the boundaries of the domain.Procedure1. Ensure that Boundary Definition is displayed. 2. Delete Inlet and Outlet from the list by right-clicking each and selecting Delete. 3. Right-click in the blank area where Inlet and Outlet were listed, then select New. 4. Set Name to: in1 5. Click OK. The boundary is created and, when selected, properties related to the boundary are displayed.Setting Boundary Data Once boundaries are created, you need to create associated data. Based on Figure 1, you will define the first inlet boundary condition to have a velocity of 2 m/s and a temperature of 315 K at one of the side inlets.Procedure1. Ensure that Boundary Data is displayed. 2. Set Boundary Type to Inlet. 3. Set Location to in1.Setting Flow Specification Once boundary data is defined, the boundary needs to have the flow specification assigned.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 37Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.49. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-PreProcedure 1. Ensure that Flow Specification is displayed.2. Set Option to Normal Speed.3. Set Normal Speed to 2 [m s^-1].Setting Temperature SpecificationOnce flow specification is defined, the boundary needs to have temperature assigned.Procedure 1. Ensure that Temperature Specification is displayed.2. Set Static Temperature to 315 [K].Reviewing the Boundary Condition DefinitionsDefining the boundary condition for in1 required several steps. Here the settings arereviewed for accuracy.Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and atemperature of 315 K at one of the side inlets.Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows:Tab SettingValueBoundary Data Boundary TypeInletLocation in1Flow SpecificationOption Normal SpeedNormal Speed 2 [m s^-1]Temperature Specification Static Temperature 315 [K]Creating the Second Inlet Boundary DefinitionBased on Figure 1, you know the second inlet boundary condition consists of a velocity of 2m/s and a temperature of 285 K at one of the side inlets. You will define that now.Procedure 1. Under Boundary Definition, right-click in the selector area and select New.2. Create a new boundary named in2 with these settings:Tab SettingValueBoundary Data Boundary TypeInletLocation in2Flow SpecificationOption Normal SpeedNormal Speed 2 [m s^-1]Temperature Specification Static Temperature 285 [K]Page 38ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.50. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-PreCreating the Outlet Boundary Definition Now that the second inlet boundary has been created, the same concepts can be applied to building the outlet boundary. 1. Create a new boundary named out with these settings:Tab Setting ValueBoundary Data Boundary Type OutletLocationoutFlow SpecificationOptionAverage Static PressureRelative Pressure 0 [Pa] 2. Click Next.Moving to General Mode There are no further boundary conditions that need to be set. All 2D exterior regions that have not been assigned to a boundary condition are automatically assigned to the default boundary condition.Procedure1. Set Operation to Enter General Mode and click Finish. The three boundary conditions are displayed in the viewer as sets of arrows at the boundary surfaces. Inlet boundary arrows are directed into the domain. Outlet boundary arrows are directed out of the domain.Setting Solver Control Solver Control parameters control aspects of the numerical solution generation process. While an upwind advection scheme is less accurate than other advection schemes, it is also more robust. This advection scheme is suitable for obtaining an initial set of results, but in general should not be used to obtain final accurate results. The time scale can be calculated automatically by the solver or set manually. The Automatic option tends to be conservative, leading to reliable, but often slow, convergence. It is often possible to accelerate convergence by applying a time scale factor or by choosing a manual value that is more aggressive than the Automatic option. In this tutorial, you will select a physical time scale, leading to convergence that is twice as fast as the Automatic option.Procedure1. Click Solver Control . 2. On the Basic Settings tab, set Advection Scheme > Option to Upwind. 3. Set Convergence Control > Fluid Timescale Control > Timescale Control toPhysical Timescale and set the physical timescale value to 2 [s]. 4. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 39Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.51. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-PreWriting the Solver (.def) FileThe simulation file, StaticMixer.cfx, contains the simulation definition in a format thatcan be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, andmodify the simulation definition. The simulation file differs from the definition file in that itcan be saved at any time while defining the simulation.Procedure 1. Click Write Solver File .The Write Solver File dialog box is displayed.2. Set File name to StaticMixer.def.3. Ensure that Start Solver Manager is selected from the drop down menu located in the top-right corner of the dialog box.4. Click Save.5. If you are notified the file already exists, click Overwrite. This file is provided in the tutorial directory and may exist in your tutorial folder if you have copied it there.6. If prompted, click Yes or Save & Quit to save StaticMixer.cfx. The definition file (StaticMixer.def) and the simulation file (StaticMixer.cfx) are created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in the Define Run dialog box.7. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41).Playing the Session File and Starting ANSYS CFX-Solver ManagerNote: This task is required only if you are starting here with the session file that was providedin the examples directory. If you have performed all the tasks in the previous steps, proceeddirectly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41).Events in ANSYS CFX-Pre can be recorded to a session file and then played back at a laterdate to drive ANSYS CFX-Pre. Session files have been created for each tutorial so that theproblems can be set up rapidly in ANSYS CFX-Pre, if desired.Procedure 1. If required, launch ANSYS Workbench.2. Click Empty Project.3. Select File > Save or click Save .4. Under File name, type: StaticMixer5. Click Save.6. Click Start CFX-Pre.7. Select Session > Play Tutorial.8. Select StaticMixer.pre.9. Click Open. A definition file is written.10. Click the CFX-Solver tab.11. Select File > Define Run.12. Under Definition File, click Browse.Page 40ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.52. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Obtaining a Solution Using ANSYS CFX-Solver 13. Select StaticMixer.def, located in the working directory.Obtaining a Solution Using ANSYS CFX-Solver Manager ANSYS CFX-Solver Manager has a visual interface that displays a variety of results and should be used when plotted data needs to be viewed during problem solving. Two windows are displayed when ANSYS CFX-Solver Manager runs. There is an adjustable split between the windows, which is oriented either horizontally or vertically depending on the aspect ratio of the entire ANSYS CFX-Solver Manager window (also adjustable). One window shows the convergence history plots and the other displays text output from ANSYS CFX-Solver. The text lists physical properties, boundary conditions and various other parameters used or calculated in creating the model. All the text is written to the output file automatically (in this case, StaticMixer_001.out).Start the Run The Define Run dialog box allows configuration of a run for processing by ANSYS CFX-Solver.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 41Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.53. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Obtaining a Solution Using ANSYS CFX-Solver When ANSYS CFX-Solver Manager is launched automatically from ANSYS CFX-Pre, all of the information required to perform a new serial run (on a single processor) is entered automatically. You do not need to alter the information in the Define Run dialog box. This is a very quick way to launch into ANSYS CFX-Solver without having to define settings and values.Procedure1. Ensure that the Define Run dialog box is displayed. 2. Click Start Run.ANSYS CFX-Solver launches and a split screen appears and displays the results of the rungraphically and as text. The panes continue to build as ANSYS CFX-Solver Manageroperates. Note: Once the second iteration appears, data begins to plot. Plotting may take a long time depending on the amount of data to process. Let the process run.Move from ANSYS CFX-Solver to ANSYS CFX-Post Once ANSYS CFX-Solver has finished, you can use ANSYS CFX-Post to review the finished results.Procedure1. When ANSYS CFX-Solver is finished, click Yes to post-process the results. After a short pause, ANSYS CFX-Post starts and ANSYS CFX-Solver Manager closes.Page 42 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.54. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostViewing the Results in ANSYS CFX-Post When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed. The viewer displays an outline of the geometry and other graphic objects. You can use the mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre.Workflow Overview This tutorial describes the following workflow for viewing results in ANSYS CFX-Post: 1. Setting the Edge Angle for a Wireframe Object (p. 44) 2. Creating a Point for the Origin of the Streamline (p. 45) 3. Creating a Streamline Originating from a Point (p. 46) 4. Rearranging the Point (p. 47) 5. Configuring a Default Legend (p. 47) 6. Creating a Slice Plane (p. 48) 7. Defining Slice Plane Geometry (p. 49) 8. Configuring Slice Plane Views (p. 49) 9. Rendering Slice Planes (p. 50) 10. Coloring the Slice Plane (p. 51) 11. Moving the Slice Plane (p. 51) 12. Adding Contours (p. 52) 13. Working with Animations (p. 53)ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 43Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.55. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostSetting the Edge Angle for a Wireframe ObjectThe outline of the geometry is called the wireframe or outline plot.By default, ANSYS CFX-Post displays only some of the surface mesh. This sometimes meansthat when you first load your results file, the geometry outline is not displayed clearly. Youcan control the amount of the surface mesh shown by editing the Wireframe object listedin the Outline.The check boxes next to each object name in the Outline control the visibility of eachobject. Currently only the Wireframe and Default Legend objects have visibility selected.The edge angle determines how much of the surface mesh is visible. If the angle betweentwo adjacent faces is greater than the edge angle, then that edge is drawn. If the edge angleis set to 0°, the entire surface mesh is drawn. If the edge angle is large, then only the mostsignificant corner edges of the geometry are drawn.For this geometry, a setting of approximately 15° lets you view the model location withoutdisplaying an excessive amount of the surface mesh.In this module you can also modify the zoom settings and view of the wireframe.Procedure 1. In the Outline, under User Locations and Plots, double-click Wireframe.Tip: While it is not necessary to change the view to set the angle, do so to explore thepractical uses of this feature.2. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select Isometric View (Z up).3. In the Wireframe details view, under Definition, click in the Edge Angle box. An embedded slider is displayed.4. Type a value of 10 [degree].5. Click Apply to update the object with the new setting.Page 44ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.56. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Notice that more surface mesh is displayed. 6. Drag the embedded slider to set the Edge Angle value to approximately 45 [degree]. 7. Click Apply to update the object with the new setting.Less of the outline of the geometry is displayed. 8. Type a value of 15 [degree]. 9. Click Apply to update the object with the new setting. 10. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select View Towards -X.Creating a Point for the Origin of the Streamline A streamline is the path that a particle of zero mass would follow through the domain.Procedure1. Select Insert > Location > Point from the main menu.You can also use the toolbars to create a variety of objects. Later modules and tutorialsexplore this further. 2. Click OK.This accepts the default name. 3. Under Definition, ensure that Method is set to XYZ. 4. Under Point, enter the following coordinates: -1, -1, 1.This is a point near the first inlet. 5. Click Apply. The point appears as a symbol in the viewer as a crosshair symbol.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 45Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.57. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostCreating a Streamline Originating from a PointWhere applicable, streamlines can trace the flow direction forwards (downstream) and/orbackwards (upstream).Procedure 1. From the main menu, select Insert > Streamline. You can also use the toolbars to create a variety of objects. Later modules and tutorials will explore this further.2. Click OK. This accepts the default name.3. Under Definition, in Start From, ensure that Point 1 is set.Tip: To create streamlines originating from more than one location, click the ellipsis iconto the right of the Start From box. This displays the Location Selector dialog box,where you can use the and keys to pick multiple locators.4. Click the Color tab.5. Set Mode to Variable.6. Set Variable to Total Temperature.7. Set Range to Local.8. Click Apply. The streamline shows the path of a zero mass particle from Point 1. The temperature is initially high near the hot inlet, but as the fluid mixes the temperature drops.Page 46ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.58. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostRearranging the Point Once created, a point can be rearranged manually or by setting specific coordinates. Tip: In this module, you may choose to display various views and zooms from the Predefined Camera option in the shortcut menu (such as Isometric View (Z up) or View Towards -X) and by using Zoom Box if you prefer to change the display.Procedure1. In Outline, under User Locations and Plots double-click Point 1.Properties for the selected user location are displayed. 2. Under Point, set these coordinates: -1, -2.9, 1. 3. Click Apply.The point is moved and the streamline redrawn. 4. In the selection tools, click Single Select. While in this mode, the normal behavior of the left mouse button is disabled. 5. In the viewer, drag Point 1 (appears as a yellow addition sign) to a new location withinthe mixer.The point position is updated in the details view and the streamline is redrawn at thenew location. The point moves normal in relation to the viewing direction. 6. Click Rotate. Tip: You can also click in the viewer area, and press the space bar to toggle between Select and Viewing Mode. A way to pick objects from Viewing Mode is to hold down + while clicking on an object with the left mouse button. 7. Under Point, reset these coordinates: -1, -1, 1. 8. Click Apply.The point appears at its original location. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X.Configuring a Default Legend You can modify the appearance of the default legend. The default legend appears whenever a plot is created that is colored by a variable. The streamline color is based on temperature; therefore, the legend shows the temperature range. The color pattern on the legend’s color bar is banded in accordance with the bands in the plot1. 1. An exception occurs when one or more bands in a contour plot represent values beyond thelegend’s range. In this case, such bands are colored using a color that is extrapolated slightlypast the range of colors shown in the legend. This can happen only when a user-specifiedrange is used for the legend.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 47Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.59. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostThe default legend displays values for the last eligible plot that was opened in the detailsview. To maintain a legend definition during an ANSYS CFX-Post session, you can create anew legend by clicking Legend .Because there are many settings that can be customized for the legend, this module allowsyou the freedom to experiment with them. In the last steps you will set up a legend, basedon the default legend, with a minor modification to the position.Tip: When editing values, you can restore the values that were present when you beganediting by clicking Reset. To restore the factory-default values, click Default.Procedure 1. Double click Default Legend View 1. The Definition tab of the default legend is displayed.2. Apply the following settingsTabSetting ValueDefinition Title ModeUser Specified Title Streamline Temp. Horizontal(Selected) Location > Y JustificationBottom3. Click Apply. The appearance and position of the legend changes based on the settings specified.4. Modify various settings in Definition and click Apply after each change.5. Select Appearance.6. Modify a variety of settings in the Appearance and click Apply after each change.7. Click Defaults.8. Click Apply.9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and Streamline 1.Since both are no longer visible, the associated legend no longer appears.Creating a Slice PlaneDefining a slice plane allows you to obtain a cross–section of the geometry.In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic objectcould be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed coloror it can vary based on the value of a variable.You already have some objects defined by default (listed in the Outline). You can viewresults on the boundaries of the static mixer by coloring each boundary object by a variable.To view results within the geometry (that is, on non-default locators), you will create newobjects.You can use the following methods to define a plane:• Three Points: creates a plane from three specified points.Page 48ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.60. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post • Point and Normal: defines a plane from one point on the plane and a normal vector to the plane. • YZ Plane, ZX Plane, and XY Plane: similar to Point and Normal, except that the normal is defined to be normal to the indicated plane.Procedure1. From the main menu, select Insert > Location > Plane or click Location > Plane. 2. In the New Plane window, type: Slice 3. Click OK.The Geometry, Color, Render, and View tabs let you switch between settings. 4. Click the Geometry tab.Defining Slice Plane Geometry You need to choose the vector normal to the plane. You want the plane to lie in the x-y plane, hence its normal vector points along the z-axis. You can specify any vector that points in the z-direction, but you will choose the most obvious (0,0,1).Procedure1. If required, under Geometry, expand Definition. 2. Under Method select Point and Normal. 3. Under Point enter 0,0,1. 4. Under Normal enter 0, 0,1. 5. Click Apply. Slice displays under User Locations and Plots. Rotate the view to see the plane.Configuring Slice Plane Views Depending on the view of the geometry, various objects may not appear because they fall in a 2D space that cannot be seen.Procedure1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z up).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 49Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.61. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostThe slice is now visible in the viewer.2. Click Zoom Box.3. Click and drag a rectangular selection over the geometry.4. Release the mouse button to zoom in on the selection.5. Click Rotate .6. Click and drag the mouse pointer down slightly to rotate the geometry towards you.7. Select Isometric View (Z up) as described earlier.Rendering Slice PlanesRender settings determine how the plane is drawn.Procedure 1. In the Details pane for Slice, select the Render tab.2. Clear Draw Faces.3. Select Draw Lines.4. Under Draw Lines change Color Mode to User Specified.5. Click the current color in Line Color to change to a different color. For a greater selection of colors, click the ellipsis to use the Select color dialog box.6. Click Apply.7. Click Zoom Box.8. Zoom in on the geometry to view it in greater detail.Page 50ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.62. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post The line segments show where the slice plane intersects with mesh element faces. The end points of each line segment are located where the plane intersects mesh element edges. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z.The image shown below can be used for comparison with tutorial 2 (in the sectionCreating a Slice Plane (p. 68)), where a refined mesh is used.Coloring the Slice Plane The Color panel is used to determine how the object faces are colored.Procedure1. Apply the following settings to SliceTab Setting ValueColor ModeVariable*VariableTemperatureRenderDraw Faces(Selected)Draw Lines(Cleared) *.You can specify the variable (in this case, temperature) used to color the graphic element. The Constant mode allows you to color the plane with a fixed color. 2. Click Apply. Hot water (red) enters from one inlet and cold water (blue) from the other.Moving the Slice Plane The plane can be moved to different locations.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 51Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.63. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostProcedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.2. Click the Geometry tab. Review the settings in Definition under Point and under Normal.3. Click Single Select .4. Click and drag the plane to a new location that intersects the domain. As you drag the mouse, the viewer updates automatically. Note that Point updates with new settings.5. Set Point settings to 0,0,1.6. Click Apply.7. Click Rotate .8. Turn off visibility for Slice by clearing the check box next to Slice in the Outline.Adding ContoursContours connect all points of equal value for a scalar variable (for example, Temperature)and help to visualize variable values and gradients. Colored bands fill the spaces betweencontour lines. Each band is colored by the average color of its two bounding contour lines(even if the latter are not displayed).Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.2. Select Insert > Contour from the main menu or click Contour.The New Contour dialog box is displayed.3. Set Name to Slice Contour.4. Click OK.5. Apply the following settingsTabSetting ValueGeometry Locations Slice VariableTemperatureRender Draw Faces(Selected)6. Click Apply.Important: The colors of 3D graphics object faces are slightly altered when lighting is on. Toview colors with highest accuracy, on the Render tab under Draw Faces clear Lighting andclick Apply.Page 52ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.64. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post The graphic element faces are visible, producing a contour plot as shown.Working with Animations Animations build transitions between views for development of video files.Workflow This tutorial follows the general workflow for creating a keyframe animation:Overview 1. Showing the Animation Dialog Box (p. 53) 2. Creating the First Keyframe (p. 53) 3. Creating the Second Keyframe (p. 54) 4. Viewing the Animation (p. 55) 5. Modifying the Animation (p. 56) 6. Saving to MPEG (p. 57)Showing the Animation Dialog Box The Animation dialog box is used to define keyframes and to export to a video file.Procedure1. Select Tools > Animation or click Animation . The Animation dialog box can be repositioned as required.Creating the First Keyframe Keyframes are required in order to produce an animation. You need to define the first viewer state, a second (and final) viewer state, and set the number of interpolated intermediate frames.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 53Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.65. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostProcedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).2. In the Outline, under User Locations and Plots, clear the visibility of Slice Contour and select the visibility of Slice.3. Select Tools > Animation or click Animation.The Animation dialog box can be repositioned as required.4. In the Animation dialog box, click New .A new keyframe named KeyframeNo1 is created. This represents the current imagedisplayed in the viewer.Creating the Second KeyframeKeyframes are required in order to produce an animation.Procedure 1. In the Outline, under User Locations and Plots, double-click Slice.2. On the Geometry tab, set Point coordinate values to (0,0,-1.99).3. Click Apply. The slice plane moves to the bottom of the mixer.4. In the Animation dialog box, click New.KeyframeNo2 is created and represents the image displayed in the Viewer.5. Select KeyframeNo1.6. Set # of Frames (located below the list of keyframes) to 20.Page 54ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.66. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post This is the number of intermediate frames used when going from KeyframeNo1 to KeyframeNo2. This number is displayed in the Frames column for KeyframeNo1. 7. Press Enter.The Frame # column shows the frame in which each keyframe appears. KeyframeNo1appears at frame 1 since it defines the start of the animation. KeyframeNo2 is at frame22 since you have 20 intermediate frames (frames 2 to 21) in between KeyframeNo1 andKeyframeNo2.Viewing the Animation More keyframes could be added, but this animation has only two keyframes (which is the minimum possible). The controls previously greyed-out in the Animation dialog box are now available. The number of intermediate frames between keyframes is listed beside the keyframe having the lowest number of the pair. The number of keyframes listed beside the last keyframe is ignored.Procedure1. Click Play the animation. The animation plays from frame 1 to frame 22. It plays relatively slowly because the slice plane must be updated for each frame.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 55Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.67. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostModifying the AnimationTo make the plane sweep through the whole geometry, you will set the starting position ofthe plane to be at the top of the mixer. You will also modify the Range properties of theplane so that it shows the temperature variation better. As the animation is played, you cansee the hot and cold water entering the mixer. Near the bottom of the mixer (where thewater flows out) you can see that the temperature is quite uniform. The new temperaturerange lets you view the mixing process more accurately than the global range used in thefirst animation.Procedure 1. Apply the following settings to SliceTab SettingValueGeometryPoint0, 0, 1.99Color Mode VariableRangeUser SpecifiedMin295 [K]Max305 [K]2. Click Apply. The slice plane moves to the top of the static mixer.Note: Do not double click in the next step.3. In the Animation dialog box, single click (do not double-click) KeyframeNo1 to select it. If you had double-clicked KeyFrameNo1, the plane and viewer states would have been redefined according to the stored settings for KeyFrameNo1. If this happens, clickUndo and try again to select the keyframe.4. Click Set Keyframe .The image in the Viewer replaces the one previously associated with KeyframeNo1.5. Double-click KeyframeNo2. The object properties for the slice plane are updated according to the settings in KeyFrameNo2.6. Apply the following settings to SliceTab SettingValueColor Mode VariableRangeUser SpecifiedMin295 [K]Max305 [K]7. Click Apply.8. In the Animation dialog box, single-click KeyframeNo2.9. Click Set Keyframe to save the new settings to KeyframeNo2.Page 56ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.68. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostSaving to MPEG By defining the geometry and then saving to MPEG, the results can be saved to a video file.Procedure1. Click More Animation Options to view the additional options. The Loop and Bounce radio buttons determine what happens when the animation reaches the last keyframe. When Loop is selected, the animation repeats itself the number of times defined by Repeat. When Bounce is selected, every other cycle is played in reverse order, starting with the second. 2. Click Save MPEG. 3. Click Browsenext to Save MPEG. 4. Under File name type: StaticMixer.mpg 5. If required, set the path location to a different folder. 6. Click Save.The MPEG file name (including path) is set. At this point, the animation has not yet beenproduced. 7. Click Previous Keyframe .Wait a moment as the display updates the keyframe display. 8. Click Play the animation. 9. If prompted to overwrite an existing movie click Overwrite.The animation plays and builds an MPEG file. 10. Click the Options button at the bottom of the Animation dialog box. In Advanced, you can see that a Frame Rate of 24 frames per second was used to create the animation. The animation you produced contains a total of 22 frames, so it takes just under 1 second to play in a media player. 11. Click Cancel to close the dialog box. 12. Close the Animation dialog box. 13. Review the animation in third–party software as required.Exiting ANSYS CFX-Post When finished with ANSYS CFX-Post, exit the current window: 1. Select File > Close to close the current file. 2. If prompted to save, click Close. 3. Return to the Project page. Select File > Close Project. 4. Select No, then close Workbench.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 57Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.69. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-PostPage 58ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.70. Tutorial 2:Flow in a Static Mixer(Refined Mesh)Introduction This tutorial includes: • Tutorial 2 Features (p. 60) • Overview of the Problem to Solve (p. 60) • Defining a Simulation using General Mode in ANSYS CFX-Pre (p. 61) • Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66) • Viewing the Results in ANSYS CFX-Post (p. 68) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 61). Sample files used by this tutorial are: • StaticMixerRefMesh.gtm • StaticMixerRef.pre • StaticMixer.def • StaticMixer_001.resANSYS CFX TutorialsPage 59ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.71. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Tutorial 2 FeaturesTutorial 2 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateFluid TypeGeneral FluidDomain Type Single DomainTurbulence Modelk-EpsilonHeat Transfer Thermal EnergyBoundary Conditions Inlet (Subsonic)Outlet (Subsonic)Wall: No-SlipWall: AdiabaticTimestepPhysical Time ScaleANSYS CFX-PostPlots PlanevolumeSlice PlaneSpherevolumeOther Viewing the Mesh In this tutorial you will learn about: • Using the General Mode of ANSYS CFX-Pre (this mode is used for more complex cases). • Rerunning a problem with a refined mesh. • Importing CCL to copy the definition of a different simulation into the current simulation. • Viewing the mesh with a Sphere volume locator and a Surface Plot. • Using a Plane Volume locator and the Mesh Calculator to analyze mesh quality.Overview of the Problem to Solve In this tutorial, you use a refined mesh to obtain a better solution to the Static Mixer problem created in Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3). You establish a general workflow for analyzing the flow of fluid into and out of a mixer. This tutorial uses a specific problem to teach the general approach taken when working with an existing mesh. You start a new simulation in ANSYS CFX-Pre and import the refined mesh. This tutorial introduces General Mode—the mode used for most tutorials—in ANSYS CFX-Pre. The physics for this tutorial are the same as for Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3); therefore, you can import the physics settings used in that tutorial to save time.Page 60 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.72. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-PreDefining a Simulation using General Mode in ANSYS CFX-Pre After having completed meshing, ANSYS CFX-Pre is used as a consistent and intuitive interface for the definition of complex CFD problems.Playing a Session File If you want to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 65). After you have played the session file, proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).Workflow Overview This section provides a brief summary of the topics so that you can see the workflow: 1. Creating a New Simulation (p. 61) 2. Importing a Mesh (p. 62) 3. Importing CCL (p. 62) 4. Viewing Domain Settings (p. 63) 5. Viewing the Boundary Condition Setting (p. 64) 6. Defining Solver Parameters (p. 64) 7. Writing the Solver (.def) File (p. 64) As an alternative to these steps, you can also review Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 65) To begin this tutorial and create a new simulation in ANSYS CFX-Pre, continue from Creating a New Simulation (p. 61).Creating a New Simulation Before importing and working with a mesh, a simulation needs to be developed using General mode. Note: Two procedures are documented. Depending on your installation of ANSYS CFX, follow either the Standalone procedure or the Workbench procedure.Procedure in 1. If required, launch ANSYS CFX-Pre.Standalone 2. Select File > New Simulation. 3. Select General in the New Simulation File dialog box and click OK. 4. Select File > Save Simulation As. 5. Under File name, type StaticMixerRef and click Save. 6. Proceed to Importing a Mesh (p. 62).Procedure in 1. If required, launch ANSYS Workbench.Workbench2. Click Empty Project.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 61Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.73. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-PreThe Project page appears displaying an unsaved project.3. Select File > Save or click Save .4. If required, set the path location to your working folder.5. Under File name, type StaticMixerRef and click Save.6. Click Start CFX-Pre under Advanced CFD on the left hand task bar.7. Select File > New Simulation.8. Click General in the New Simulation File window, and then click OK.9. Select File > Save Simulation As.10. Under File name, type StaticMixerRef and click Save.Importing a MeshAt least one mesh must be imported before physics are applied.An assembly is a group of mesh regions that are topologically connected. Each assemblycan contain only one mesh, but multiple assemblies are permitted. The Mesh tree shows theregions in Assembly in a tree structure. The level below Assembly displays 3D regions andthe level below each 3D region shows the 2D regions associated with it. The check box nextto each item in the Mesh tree indicates the visibility status of the object in the viewer; youcan click these to toggle visibility.Procedure 1. Select File > Import Mesh or right-click Mesh and select Import Mesh.2. In the Import Mesh dialog box, select StaticMixerRefMesh.gtm from your working directory. This is a mesh that is more refined than the one used in Tutorial 1.3. Click Open.4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.Importing CCLSince the physics for this simulation is very similar to that for Tutorial 1, you can save timeby importing the settings used there.The CCL contains settings that reference mesh regions. For example, the outlet boundarycondition references the mesh region named out. In this tutorial, the name of the meshregions are the same as in Tutorial 1, so you can import the CCL without error.The physics for a simulation can be saved to a CCL (CFX Command Language) file at any timeby selecting File > Export CCL. However, a number of other files can also be used as sourcesto import CCL including:• Simulation files (*.cfx)• Results files (*.res)• Definition files(*.def)Note: If you import CCL that references non-existent mesh regions, you will get errors.Page 62ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.74. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-PreProcedure1. Select File > Import CCL.The Import CCL dialog box appears. 2. Under Import Method, select Append.Replace is useful if you have defined physics and want to update or replace them withnewly imported physics. 3. Under File type, select CFX-Solver Files (*def *res). 4. Select StaticMixer.def created in Tutorial 1. If you did not work through Tutorial 1,you can copy this file from the examples directory. 5. Click Open. 6. Select the Outline tab. Tip: To select Outline you may need to click the navigation icons next to the tabs to move ‘forward’ or ‘backward’ through the various tabs. The tree view displays a summary of the current simulation in a tree structure. Some items may be recognized from Tutorial 1—for example the boundary condition objects in1, in2, and out.Viewing Domain Settings It is useful to review the options available in General Mode. Various domain settings can be set. These include: • General Options Specifies the location of the domain, coordinate frame settings and the fluids/solids that are present in the domain. You also reference pressure, buoyancy and whether the domain is stationary or rotating. Mesh motion can also be set. • Fluid Models Sets models that apply to the fluid(s) in the domain, such as heat transfer, turbulence, combustion, and radiation models. An option absent in Tutorial 1 is Turbulent Wall Functions, which is set to Scalable. Wall functions model the flow in the near-wall region. For the k-epsilon turbulence model, you should always use scalable wall functions. • Initialization Sets the initial conditions for the current domain only. This is generally used when multiple domains exist to allow setting different initial conditions in each domain, but can also be used to initialize single-domain simulations. Global initialization allows the specification of initial conditions for all domains that do not have domain-specific initialization.Procedure1. On the Outline tree view, under Simulation, double-click Default Domain.The domain Default Domain is opened for editing. 2. Click General Options and review, but do not change, the current settings. 3. Click Fluid Models and review, but do not change, the current settings. 4. Click Initialization and review, but do not change, the current settings. 5. Click Close.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 63Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.75. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-PreViewing the Boundary Condition SettingFor the k-epsilon turbulence model, you must specify the turbulent nature of the flowentering through the inlet boundary. For this simulation, the default setting of Medium(Intensity = 5%) is used. This is a sensible setting if you do not know the turbulenceproperties of the incoming flow.Procedure 1. Under Default Domain, double-click in1.2. Click the Boundary Details tab and review the settings for Flow Regime, Mass and Momentum, Turbulence and Heat Transfer.3. Click Close.Defining Solver ParametersSolver Control parameters control aspects of the numerical-solution generation process.In Tutorial 1 you set some solver control parameters, such as Advection Scheme andTimescale Control, while other parameters were set automatically by ANSYS CFX-Pre.In this tutorial, High Resolution is used for the advection scheme. This is more accuratethan the Upwind Scheme used in Tutorial 1. You usually require a smaller timestep whenusing this model. You can also expect the solution to take a higher number of iterations toconverge when using this model.Procedure 1. Select Insert > Solver > Solver Control from the main menu or click Solver Control .2. Apply the following Basic SettingsSettingValueAdvection Scheme > OptionHigh ResolutionConvergence Control > Max. Iterations* 150Convergence Control > Fluid Timescale Control >Physical TimescaleTimescale ControlConvergence Control > Fluid Timescale Control > Physical 0.5 [s]Timescale *.If your solution does not meet the convergence criteria after this number of timesteps, the ANSYS CFX-Solver will stop.3. Click Apply.4. Click the Advanced Options tab.5. Ensure that Global Dynamic Model Control is selected.6. Click OK.Writing the Solver (.def) FileOnce all boundaries are created you move from ANSYS CFX-Pre into ANSYS CFX-Solver.Page 64ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.76. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-Pre The simulation file—StaticMixerRef.cfx—contains the simulation definition in a format that can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and modify the simulation definition. The simulation file differs from the definition file in two important ways: • The simulation file can be saved at any time while defining the simulation. • The definition file is an encapsulated set of meshes and CCL defining a solver run, and is a subset of the data in the simulation file.Procedure1. Click Write Solver File . The Write Solver File dialog box is displayed. 2. If required, set the path to your working directory. 3. Apply the following settings:Setting ValueFile name StaticMixerRef.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 4. Ensure Start Solver Manager is selected and click Save. 5. If you are notified that the file already exists, click Overwrite. 6. If prompted, click Yes or Save & Quit to save StaticMixerRef.cfx.The definition file (StaticMixerRef.def) and the simulation file(StaticMixerRef.cfx) are created. ANSYS CFX-Solver Manager automatically startsand the definition file is set in the Definition File box of Define Run. 7. Proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).Playing the Session File and Starting ANSYS CFX-Solver Manager If you have performed all the tasks in the previous steps, proceed directly to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66). Two procedures are documented. Depending on your installation of ANSYS CFX follow either the standalone procedure or the ANSYS Workbench procedure.Procedure in 1. If required, launch ANSYS CFX-Pre.Standalone 2. Select Session > Play Tutorial. 3. Select StaticMixerRef.pre. 4. Click Open.A definition file is written. 5. Select File > Quit. 6. Launch ANSYS CFX-Solver Manager from CFX Launcher. 7. After ANSYS CFX-Solver starts, select File > Define Run. 8. Under Definition File, click Browse. 9. Select StaticMixerRef.def, located in the working directory.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 65Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.77. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Obtaining a Solution Using Interpolation with ANSYS CFX-Solver10. Proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66).Procedure in1. If required, launch ANSYS Workbench.ANSYS 2. Click Empty Project.Workbench3. Select File > Save or click Save .4. Under File name, type StaticMixerRef and click Save.5. Click Start CFX-Pre.6. Select Session > Play Tutorial.7. Select StaticMixerRef.pre.8. Click Open. A definition file is written.9. Click the CFX-Solver tab.10. Select File > Define Run.11. Under Definition File, click Browse.12. Select StaticMixerRef.def, located in the working directory.Obtaining a Solution Using Interpolation with ANSYSCFX-SolverTwo windows are displayed when ANSYS CFX-Solver Manager runs. There is an adjustablesplit between the windows which is oriented either horizontally or vertically, depending onthe aspect ratio of the entire ANSYS CFX-Solver Manager window (also adjustable).Workflow OverviewThis section provides a brief summary of the topics to follow as a general workflow:1. Interpolating the Results and Starting the Run (p. 66)2. Confirming Results (p. 67)3. Moving from ANSYS CFX-Solver to ANSYS CFX-Post (p. 67)Interpolating the Results and Starting the RunIn the ANSYS CFX-Solver Manager, Define Run is visible and Definition File hasautomatically been set to the definition file from ANSYS CFX-Pre: StaticMixerRef.def.You want to make use of the results from Tutorial 1, but the two meshes are not identical.The initial values file needs to have its data interpolated onto the new mesh associated withthe definition file.The ANSYS CFX-Solver supports automatic interpolation that will be used in the followingsteps:Page 66ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.78. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Obtaining a Solution Using Interpolation with ANSYS CFX-Solver The values from StaticMixer_001.res will be interpolated onto the definition file’s mesh when the run is started. The results from StaticMixer_001.res will be used as the initial guess for this simulation (rather than Solver defaults) because you have set the initialization for all variables in ANSYS CFX-Pre to Automatic or Automatic with Value.Procedure1. Under Initial Values File, click Browse . 2. Select the results file from Tutorial 1: StaticMixer_001.resIf you did not complete the first tutorial, you can use StaticMixer_001.res from yourworking directory. 3. Click Open. 4. Select Interpolate Initial Values onto Def File Mesh. 5. Click Start Run. Note: The message Finished interpolation successfully appears relatively quickly. Convergence information is plotted once the second outer loop iteration is complete.Confirming Results When interpolation is successful, specific information appears in the text screen of ANSYS CFX-Solver. To confirm that the interpolation was successful, look in the text pane in ANSYS CFX-Solver Manager. The following text appears before the convergence history begins: +---------------------------------------------------------+ | Initial Conditions Supplied by Fields in the Input Files +---------------------------------------------------------+ This lists the variables that were interpolated from the results file. After the final iteration, a message similar to the following content appears: CFD Solver finished: Tue Oct 19 08:06:45 2004 CFD Solver wall clock seconds: 1.7100E+02 Execution terminating: all residual are below their target criteria This indicates that ANSYS CFX-Solver has successfully calculated the solution for the problem to the specified accuracy or has run out of coefficient loops.Procedure1. When the run finishes and asks if you want to post-process the results, click No to keepANSYS CFX-Solver open. Review the results on the Out File tab for details on the runresults.Moving from ANSYS CFX-Solver to ANSYS CFX-Post Once ANSYS CFX-Solver has finished, you can use ANSYS CFX-Post to review the finished results.Procedure1. Select Tools > Post–Process Results or click Post–Process Resultsin the toolbar. 2. If using ANSYS CFX-Solver in Standalone Mode, select Shut down Solver Manager.This forces Standalone ANSYS CFX-Solver to close when finished. This option is notrequired in Workbench. 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 67Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.79. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-PostAfter a short pause, ANSYS CFX-Post starts.Viewing the Results in ANSYS CFX-PostIn the following sections, you will explore the differences between the mesh and the resultsfrom this tutorial and tutorial 1.Creating a Slice PlaneMore information exists for use by ANSYS CFX-Post in this tutorial than in Tutorial 1 becausethe slice plane is more detailed.Once a new slice plane is created it can be compared with Tutorial 1. There are threenoticeable differences between the two slice planes.• Around the edges of the mixer geometry there are several layers of narrow rectangles.This is the region where the mesh contains prismatic elements (which are created asinflation layers). The bulk of the geometry contains tetrahedral elements.• There are more lines on the plane than there were in Tutorial 1. This is because the sliceplane intersects with more mesh elements.• The curves of the mixer are smoother than in Tutorial 1 because the finer mesh betterrepresents the true geometry.Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).2. From the main menu, select Insert > Location > Plane or under Location, click Plane.3. In the Insert Plane dialog box, type Slice and click OK. The Geometry, Color, Render and View tabs let you switch between settings.4. Apply the following settingsTab SettingValueGeometryDomainsDefault DomainDefinition > MethodXY PlaneDefinition > Z 1 [m]RenderDraw Faces (Cleared)Draw Lines (Selected)5. Click Apply.6. Right-click a blank area in the viewer and select Predefined Camera > View Towards -Z.7. Click Zoom Box.8. Zoom in on the geometry to view it in greater detail.Page 68ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.80. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post Compare the on-screen image with the equivalent picture from tutorial 1 (in the section Rendering Slice Planes (p. 22)).Coloring the Slice Plane Here, you will color the plane by temperature.Procedure1. Apply the following settingsTab SettingValueColor Mode*VariableVariable TemperatureRangeGlobalRenderDraw Faces (Selected)Draw Lines (Cleared) *.A mode setting of Constant would allow you to color the plane with a fixed color. 2. Click Apply.Loading Results from Tutorial 1 for Comparison In ANSYS CFX-Post, you may load multiple results files into the same instance for comparison.Procedure1. To load the results file from Tutorial 1, select File > Load Results or click Load Results . 2. Be careful not to click Open until instructed to do so. In the Load Results File dialogbox, select StaticMixer_001.res in the examples directory or from yourworking directory if it has been copied.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 69Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.81. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post3. On the right side of the dialog box, there are two frames. Under Results file option, select Add to current results.4. Select the Offset in Y direction check box.5. Under Additional actions, ensure that the Clear user state before loading check box is cleared.6. Click Open to load the results. In the tree view, there is now a second group of domains, meshes and boundary conditions with the heading StaticMixer_001.7. Double-click the Wireframe object under User Locations and Plots.8. In the Definition tab, set Edge Angle to 5 [degree].9. Click Apply.10. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z up).Both meshes are now displayed in a line along the Y axis. Notice that one mesh is of ahigher resolution than the other.11. Set Edge Angle to 30 [degree].12. Click Apply.Creating a Second Slice PlaneProcedure 1. In the tree view, right-click the plane named Slice and select Duplicate.2. Click OK to accept the default name Slice 1.3. In the tree view, double-click the plane named Slice 1.4. On the Geometry tab, set Domains to Default Domain 1.5. On the Color tab, ensure that Range is set to Global.6. Click Apply.7. Double-click Slice and make sure that Range is set to Global.Comparing Slice Planes using Multiple ViewsProcedure 1. Select the option with the two vertical rectangles. Notice that the Viewer now has two separate views.The visibility status of each object is maintained separately for each view or figure thatcan be displayed in a given viewport. This allows some planes to be shown while othersare hidden.Page 70ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.82. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post 2. Click in the viewport that is set to show View 1, then clear the visibility check box forSlice in the Outline tree view and ensure that the visibility check box for Slice 1 isselected. 3. Click in the viewport that is set to show View 2, then select the visibility check box forSlice and ensure that the visibility check box for Slice 1 is cleared. 4. In the tree view, double-click StaticMixer_001 and clear Apply Translation. 5. Click Apply. 6. In the viewer toolbar, click Synchronise Active Views . Notice that both views move in the same way and are zoomed in at the same level. 7. Right-click in the viewer and select Predefined Camera > View Towards -Z.Note the difference in temperature distribution. 8. To return to a single viewport, select the option with a single rectangle. 9. Right-click Slice 1 in the tree view and select Delete. 10. Ensure that the visibility check box for Slice is cleared. 11. Right-click StaticMixer_001 in the tree view and select Unload.Viewing the Surface Mesh on the Outlet In this part of the tutorial, you will view the mesh on the outlet. You will see five layers of inflated elements against the wall. You will also see the triangular faces of the tetrahedral elements closer to the center of the outlet.Procedure1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z up). 2. In the tree view, ensure that the visibility check box for StaticMixerRef_001 >Default Domain > out is selected, then double-click out to open it for editing.Since the boundary location geometry was defined in ANSYS CFX-Pre, the details viewdoes not display a Geometry tab as it did for the planes. 3. Apply the following settingsTab Setting ValueRenderDraw Faces(Cleared)Draw Lines(Selected)Color ModeUser SpecifiedLine Color(Select any light color) 4. Click Apply.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 71Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.83. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post5. Click Zoom Box.6. Zoom in on the geometry to view out in greater detail.7. Click Rotate on the Viewing Tools toolbar.8. Rotate the image as required to clearly see the mesh.Looking at the Inflated Elements in Three DimensionsTo show more clearly what effect inflation has on the shape of the elements, you will usevolume objects to show two individual elements. The first element that will be shown is anormal tetrahedral element; the second is a prismatic element from an inflation layer of themesh.Leave the surface mesh on the outlet visible to help see how surface and volume meshes arerelated.Procedure 1. From the main menu, select Insert > Location > Volume or, under Location click Volume.2. In the Insert Volume dialog box, type Tet Volume and click OK.3. Apply the following settingsTab SettingValueGeometryDefinition > MethodSphereDefinition > Point * 0.08, 0, -2Definition > Radius0.14 [m]Definition > ModeBelow IntersectionInclusive† (Cleared)Color ColorRedRenderDraw Faces > Transparency0.3Draw Lines (Selected)Draw Lines > Line Width1Draw Lines > Color ModeUser SpecifiedDraw Lines > Line ColorGrey *.The z slider’s minimum value corresponds to the minimum z value of the entire geometry, which, in this case, occurs at the outlet. †.Only elements that are entirely contained within the sphere volume will be included.4. Click Apply to create the volume object.5. Right-click Tet Volume and choose Duplicate.6. In the Duplicate Tet Volume dialog box, type Prism Volume and click OK.7. Double-click Prism Volume.8. Apply the following settingsPage 72ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.84. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-PostTab Setting ValueGeometryDefinition > Point-0.22, 0.4, -1.85Definition > Radius 0.206 [m]Color Color Orange 9. Click Apply.Viewing the Surface Mesh on the Mixer BodyProcedure1. Double-click the Default Domain Default object. 2. Apply the following settingsTab Setting ValueRenderDraw Faces(Selected)Draw Lines(Selected)Line Width2 3. Click Apply.Viewing the Layers of Inflated Elements on a Plane You will see the layers of inflated elements on the wall of the main body of the mixer. Within the body of the mixer, there will be many lines that are drawn wherever the face of a mesh element intersects the slice plane.Procedure1. From the main menu, select Insert > Location > Plane or under Location, click Plane. 2. In the Insert Plane dialog box, type Slice 2 and click OK. 3. Apply the following settingsTab Setting ValueGeometryDefinition > Method YZ PlaneDefinition > X0 [m]RenderDraw Faces(Cleared)Draw Lines(Selected) 4. Click Apply. 5. Turn off the visibility of all objects except Slice 2. 6. To see the plane clearly, right-click in the viewer and select Predefined Camera > ViewTowards -X.Viewing the Mesh Statistics You can use the Report Viewer to check the quality of your mesh. For example, you can load a .def file into ANSYS CFX-Post and check the mesh quality before running the .def file in the solver.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 73Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.85. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-PostProcedure 1. Click the Report Viewer tab (located below the viewer window). A report appears. Look at the table shown in the “Mesh Report” section.2. Double-click Report > Mesh Report in the Outline tree view.3. In the Mesh Report details view, select Statistics > Maximum Face Angle.4. Click Refresh Preview.Note that a new table, showing the maximum face angle for all elements in the mesh,has been added to the “Mesh Report” section of the report. The maximum face angle isreported as 148.95°.As a result of generating this mesh statistic for the report, a new variable, Maximum FaceAngle, has been created and stored at every node. This variable will be used in the nextsection.Viewing the Mesh Elements with Largest Face AngleIn this section, you will visualize the mesh elements that have a Maximum Face Angle valuegreater than 140°.Procedure 1. Click the 3D Viewer tab (located below the viewer window).2. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).3. In the Outline tree view, select the visibility check box of Wireframe.4. From the main menu, select Insert > Location > Volume or under Location, click Volume.5. In the Insert Volume dialog box, type Max Face Angle Volume and click OK.6. Apply the following settingsTab SettingValueGeometryDefinition > MethodIsovolumeDefinition > VariableMaximum Face Angle*Definition > ModeAbove ValueDefinition > Value 140 [degree]Inclusive† (Selected) *.Select Maximum Face Angle from the larger list of variables available by clicking to the right of the Variable box. †.This includes any elements that have at least one node with a variable value greater than or equal to the given value.7. Click Apply.The volume object appears in the viewer.Page 74ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.86. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-PostViewing the Mesh Elements with Largest Face Angle Using a Point Next, you will create a point object to show a node that has the maximum value of Maximum Face Angle. The point object will be represented by a 3D yellow crosshair symbol. In order to avoid obscuring the point object with the volume object, you may want to turn off the visibility of the latter.Procedure1. From the main menu, select Insert > Location > Point or under Location, click Point. 2. Click OK to use the default name. 3. Apply the following settingsTab Setting ValueGeometryDefinition > Method Variable MaximumDefinition > Location Default DomainDefinition > Variable Maximum Face AngleSymbolSymbol Size 2 4. Click Apply.Quitting ANSYS CFX-Post Two procedures are documented. Depending on your installation of ANSYS CFX, follow either the standalone procedure or the ANSYS Workbench procedure.Procedure in 1. When you are finished, select File > Quit to exit ANSYS CFX-Post.Standalone 2. Click Quit if prompted to save.Procedure in 1. When you are finished, select File > Close to close the current file.Workbench2. Click Close if prompted to save. 3. Return to the Project page. Select File > Close Project. 4. Select No, then close Workbench.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 75Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.87. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-PostPage 76ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.88. Tutorial 3:Flow in a Process InjectionMixing PipeIntroduction This tutorial includes: • Tutorial 3 Features (p. 78) • Overview of the Problem to Solve (p. 78) • Defining a Simulation using General Mode in ANSYS CFX-Pre (p. 79) • Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87) • Viewing the Results in ANSYS CFX-Post (p. 88) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 79). Sample files referenced by this tutorial include: • InjectMixer.pre • InjectMixer_velocity_profile.csv • InjectMixerMesh.gtmANSYS CFX TutorialsPage 77ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.89. Tutorial 3: Flow in a Process Injection Mixing Pipe: Tutorial 3 FeaturesTutorial 3 Features This tutorial addresses the following features of ANSYS CFX.Component FeatureDetailsANSYS CFX-Pre User ModeGeneral ModeSimulation TypeSteady StateFluid Type General FluidDomain TypeSingle DomainTurbulence Model k-EpsilonHeat TransferThermal EnergyBoundary ConditionsBoundary Profile visualization Inlet (Profile) Inlet (Subsonic) Outlet (Subsonic) Wall: No-Slip Wall: AdiabaticCEL (CFX Expression Language)Timestep Physical Time ScaleANSYS CFX-PostPlotsdefault Locators Outline Plot (Wireframe) Slice Plane StreamlineOtherChanging the Color Range Expression Details View Legend Viewing the Mesh In this tutorial you will learn about: • Applying a profile boundary condition using data stored in a file. • Visualizing the velocity on a boundary in ANSYS CFX-Pre. • Using the CFX Expression Language (CEL) to describe temperature dependent fluid properties in ANSYS CFX-Pre. • Using the k-epsilon turbulence model. • Using streamlines in ANSYS CFX-Post to track flow through the domain.Overview of the Problem to Solve In this tutorial, you establish a general workflow for analyzing the flow of fluid into and out of an injection pipe. This tutorial is important because it uses a specific problem to teach the general approach taken when working with an existing mesh.Page 78 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.90. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre The injection mixing pipe, common in the process industry, is composed of two pipes: one with a larger diameter than the other. Analyzing and optimizing the mixing process is often critical for many chemical processes. CFD is useful not only in identifying problem areas (where mixing is poor), but also in testing new designs before they are implemented. The geometry for this example consists of a circular pipe of diameter 1.0 m with a 90° bend, and a smaller pipe of diameter 0.3 m which joins with the main pipe at an oblique angle. Figure 1 Injection Mixing Pipe0.5 m/s φ=1.0 m285.0 Kφ=0.3 m 5.0 m/s 315.0 KDefining a Simulation using General Mode in ANSYS CFX-Pre After having completed meshing, ANSYS CFX-Pre is used as a consistent and intuitive interface for the definition of complex CFD problems.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87). After you have played the session file, proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87).Workflow Overview This section provides a brief summary of the topics to follow as a general workflow: 1. Creating a New Simulation (p. 80) 2. Importing a Mesh (p. 80) 3. Setting Temperature-Dependent Material Properties (p. 81) 4. Plotting an Expression (p. 82)ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 79Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.91. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre5. Evaluating an Expression (p. 82)6. Modify Material Properties (p. 82)7. Creating the Domain (p. 82)8. Creating the Side Inlet Boundary Conditions (p. 83)9. Creating the Main Inlet Boundary Conditions (p. 84)10. Creating the Main Outlet Boundary Condition (p. 85)11. Setting Initial Values (p. 85)12. Setting Solver Control (p. 85)13. Writing the Solver (.def) File (p. 86)Creating a New SimulationBefore importing and working with a mesh, a simulation needs to be started using GeneralMode.Note: Two procedures are documented. Depending on your installation of ANSYS CFXfollow either the Standalone procedure or the Workbench procedure.Procedure in1. If required, launch ANSYS CFX-Pre.Standalone2. Select File > New Simulation.3. Ensure General is selected and click OK.4. Select File > Save Simulation As.5. Under File name, type InjectMixer.6. Click Save.7. Proceed to Importing a Mesh (p. 80).Procedure in1. If required, launch ANSYS Workbench.Workbench 2. Click Empty Project. The Project page will appear displaying an unsaved project.3. Select File > Save or click Save .4. If required, set the path location to your working folder.5. Under File name, type InjectMixer.6. Click Save.7. Click Start CFX-Pre under Advanced CFD on the left hand task bar.8. Select File > New Simulation.9. Click General in the New Simulation File window and then click OK.10. Select File > Save Simulation As.11. Under File name, type InjectMixer.12. Click Save.Importing a MeshAn assembly is a group of mesh regions that are topologically connected. Each assemblycan contain only one mesh, but multiple assemblies are permitted.Page 80ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.92. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-PreProcedure1. Select File > Import Mesh. 2. From your tutorial directory, select InjectMixerMesh.gtm. 3. Click Open. 4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Y up) from the shortcut menu.Setting Temperature-Dependent Material Properties You will create an expression for viscosity as a function of temperature and then use this expression to modify the properties of the library material: Water. Viscosity will be made to vary linearly with temperature between the following conditions: • µ =1.8E-03 N s m-2 at T=275.0 K • µ =5.45E-04 N s m-2 at T=325.0 K The variable T (Temperature) is a ANSYS CFX System Variable recognized by ANSYS CFX-Pre, denoting static temperature. All variables, expressions, locators, functions, and constants can be viewed by double-clicking the appropriate entry (such as Additional Variables or Expressions) in the tree view. All expressions must have consistent units. You should be careful if using temperature in an expression with units other than [K]. The Expressions tab lets you define, modify, evaluate, plot, copy, delete and browse through expressions used within ANSYS CFX-Pre.Procedure1. From the main menu, select Insert > Expressions, Functions and Variables >Expression. 2. In the New Expression dialog box, type Tupper. 3. Click OK.The details view for the Tupper equation is displayed. 4. Under Definition, type 325 [K]. 5. Click Apply to create the expression.The expression is added to the list of existing expressions. 6. Right-click in the Expressions workspace and select New. 7. In the New Expression dialog box, type Tlower. 8. Click OK. 9. Under Definition, type 275 [K]. 10. Click Apply to create the expression. The expression is added to the list of existing expressions. 11. Create expressions for Visupper, Vislower and VisT using the following values.NameDefinitionVisupper5.45E-04 [N s m^-2]Vislower1.8E-03 [N s m^-2]VisTVislower+(Visupper-Vislower)*(T-Tlower)/(Tupper-Tlower)ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 81Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.93. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-PrePlotting an ExpressionProcedure 1. Right-click VisT in the Expressions tree view, and then select Edit. The Expressions details view for VisT appears.Tip: Alternatively, double-clicking the expression also opens the Expressions detailsview.2. Click the Plot tab and apply the following settingsTab SettingValuePlotNumber of Points 10T(Selected)Start of Range 275 [K]End of Range 325 [K]3. Click Plot Expression.A plot showing the variation of the expression VisT with the variable T is displayed.Evaluating an ExpressionProcedure 1. Click the Evaluate tab.2. In T, type 300 [K]. This is between the start and end range defined in the last module.3. Click Evaluate Expression.The value of VisT for the given value of T appears in the Value field.Modify Material PropertiesDefault material properties (such as those of Water) can be modified when required.Procedure 1. Click the Outline tab.2. Double click Water under Materials to display the Basic Settings tab.3. Click the Material Properties tab.4. Expand Transport Properties.5. Select Dynamic Viscosity.6. Under Dynamic Viscosity, click in Dynamic Viscosity.7. Click Enter Expression.8. Enter the expression VisT into the data box.9. Click OK.Creating the DomainThe domain will be set to use the thermal energy heat transfer model, and the k-ε(k-epsilon) turbulence model.Page 82ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.94. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre Both General Options and Fluid Models are changed in this module. The Initialization tab is for setting domain-specific initial conditions, which are not used in this tutorial. Instead, global initialization is used to set the starting conditions.Procedure1. Select Insert > Domain from the main menu or click Domain. 2. In the Insert Domain dialog box, type InjectMixer. 3. Click OK. 4. Apply the following settingsTab SettingValueGeneral Options Basic Settings > LocationB1.P3Basic Settings > Fluids List WaterDomain Models > Pressure > 0 [atm]Reference Pressure 5. Click Fluid Models. 6. Apply the following settingsSetting ValueHeat Transfer > OptionThermal Energy 7. Click OK.Creating the Side Inlet Boundary Conditions The side inlet boundary condition needs to be defined.Procedure1. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 2. Set Name to side inlet. 3. Click OK. 4. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation side inletBoundary DetailsMass and Momentum > Option Normal SpeedNormal Speed 5 [m s^-1]Heat Transfer > Option Static TemperatureStatic Temperature 315 [K] 5. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 83Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.95. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-PreCreating the Main Inlet Boundary ConditionsThe main inlet boundary condition needs to be defined. This inlet is defined using a velocityprofile found in the example directory. Profile data needs to be initialized before theboundary condition can be created.You will create a plot showing the velocity profile data, marked by higher velocities near thecenter of the inlet, and lower velocities near the inlet walls.Procedure 1. Select Tools > Initialize Profile Data.2. Under Data File, click Browse.3. From your working directory, select InjectMixer_velocity_profile.csv.4. Click Open.5. Click OK. The profile data is read into memory.6. Select Insert > Boundary Condition from the main menu or click Boundary Condition.7. Set name Name to main inlet.8. Click OK.9. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation main inletProfile Boundary Conditions (Selected)> Use Profile DataProfile Boundary Setup > main inletProfile Name10. Click Generate Values.This causes the profile values of U, V, W to be applied at the nodes on the main inletboundary, and U, V, W entries to be made in Boundary Details. To later modify thevelocity values at the main inlet and reset values to those read from the BC Profile file,revisit Basic Settings for this boundary condition and click Generate Values.11. Apply the following settingsTab SettingValueBoundary DetailsFlow Regime > Option SubsonicTurbulence > OptionMedium (Intensity = 5%)Heat Transfer > Option Static TemperatureStatic Temperature 285 [K]Plot OptionsBoundary Contour (Selected)Profile Variable W12. Click OK.Page 84ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.96. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre 13. Zoom into the main inlet to view the inlet velocity contour.Creating the Main Outlet Boundary Condition In this module you create the outlet boundary condition. All other surfaces which have not been explicitly assigned a boundary condition will remain in the InjectMixer Default object, which is shown in the tree view. This boundary condition uses a No-Slip Adiabatic Wall by default.Procedure1. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 2. Set Name to outlet. 3. Click OK. 4. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeOutletLocation outletBoundary DetailsFlow Regime > Option SubsonicMass and Momentum > Option Average Static PressureRelative Pressure0 [Pa] 5. Click OK.Setting Initial ValuesProcedure1. Click Global Initialization . 2. Select Turbulence Eddy Dissipation. 3. Click OK.Setting Solver ControlProcedure1. Click Solver Control . 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 85Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.97. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-PreTab SettingValueBasic SettingsAdvection Scheme > Option Specified Blend FactorAdvection Scheme > Blend 0.75FactorConvergence Control > Max. 50IterationsConvergence Control >Physical TimescaleFluid Timescale Control >Timescale ControlConvergence Control >2 [s]Fluid Timescale Control >Physical TimescaleConvergence Criteria > RMSResidual TypeConvergence Criteria > 1.E-4*Residual Target *.An RMS value of at least 1.E-5 is usually required for adequate convergence, but the default value is sufficient for demonstration purposes.3. Click OK.Writing the Solver (.def) FileOnce the problem has been defined you move from General Mode into ANSYS CFX-Solver.Procedure 1. Click Write Solver File .The Write Solver File dialog box appears.2. Apply the following settings:Setting ValueFile name InjectMixer.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode.3. Ensure Start Solver Manager is selected and click Save.4. If you are notified the file already exists, click Overwrite. This file is provided in the tutorial directory and may exist in your working folder if you have copied it there.5. If prompted, click Yes or Save & Quit to save InjectMixer.cfx. The definition file (InjectMixer.def), mesh file (InjectMixer.gtm) and the simulation file (InjectMixer.cfx) are created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in the Definition File box of Define Run.6. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87).Page 86ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.98. Tutorial 3: Flow in a Process Injection Mixing Pipe: Obtaining a Solution Using ANSYS CFX-Solver ManagerPlaying the Session File and Starting ANSYS CFX-Solver Manager If you have performed all the tasks in the previous steps, proceed directly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87). Two procedures are documented. Depending on your installation of ANSYS CFX, follow either the standalone procedure or the ANSYS Workbench procedure.Procedure in 1. If required, launch ANSYS CFX-Pre.Standalone 2. Select Session > Play Tutorial. 3. Select InjectMixer.pre. 4. Click Open.A definition file is written. 5. Select File > Quit. 6. Launch ANSYS CFX-Solver Manager from CFX Launcher. 7. After ANSYS CFX-Solver starts, select File > Define Run. 8. Under Definition File, click Browse. 9. Select InjectMixer.def, located in the working directory. 10. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87).Procedure in 1. If required, launch ANSYS Workbench.ANSYS2. Click Empty Project.Workbench 3. Select File > Save or click Save . 4. Under Filename, type InjectMixer. 5. Click Save. 6. Click Start CFX-Pre. 7. Select Session > Play Tutorial. 8. Select InjectMixer.pre. 9. Click Open.A definition file is written. 10. Click the CFX-Solver tab. 11. Select File > Define Run. 12. Under Definition File, click Browse . 13. Select InjectMixer.def, located in the working directory.Obtaining a Solution Using ANSYS CFX-Solver Manager At this point, ANSYS CFX-Solver Manager is running, and the Define Run dialog box is displayed, with the definition file set. 1. Click Start Run. 2. Click No to close the message box that appears when the run ends.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 87Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.99. Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-PostMoving from ANSYS CFX-Solver Manager to ANSYS CFX-Post 1. Select Tools > Post–Process Results or click Post–Process Results . 2. If using ANSYS CFX-Solver Manager in standalone mode, optionally select Shut downSolver Manager. 3. Click OK.Viewing the Results in ANSYS CFX-Post When ANSYS CFX-Post starts, the viewer and Outline workspace display by default.Workflow Overview This section provides a brief summary of the topics to follow as a general workflow: 1. Modifying the Outline of the Geometry (p. 88) 2. Creating and Modifying Streamlines (p. 88) 3. Modifying Streamline Color Ranges (p. 89) 4. Coloring Streamlines with a Constant Color (p. 89) 5. Duplicating and Modifying a Streamline Object (p. 90) 6. Examining Turbulent Kinetic Energy (p. 90)Modifying the Outline of the Geometry Throughout this and the following examples, use your mouse and the Viewing Tools toolbar to manipulate the geometry as required at any time.Procedure1. In the tree view, double click Wireframe. 2. Set the Edge Angle to 15 [degree]. 3. Click Apply.Creating and Modifying Streamlines When you complete this module you will see streamlines (mainly blue and green) starting at the main inlet of the geometry and proceeding to the outlet. Above where the side pipe meets the main pipe, there is an area where the flow re-circulates rather than flowing roughly tangent to the direction of the pipe walls.Procedure1. Select Insert > Streamline from the main menu or click Streamline . 2. Under Name, type MainStream. 3. Click OK. 4. Apply the following settingsPage 88 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.100. Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-PostTab Setting ValueGeometryType3D StreamlineDefinition > Start From main inlet 5. Click Apply. 6. Right-click a blank area in the viewer, select Predefined Camera from the shortcutmenu, then select Isometric View (Y up). The pipe is displayed with the main inlet in the bottom right of the viewer.Modifying Streamline Color Ranges You can change the appearance of the streamlines using the Range setting on the Color tab.Procedure1. Under User Locations and Plots, modify the streamline object MainStream byapplying the following settingsTab Setting ValueColor Range Local 2. Click Apply.The color map is fitted to the range of velocities found along the streamlines. Thestreamlines therefore collectively contain every color in the color map. 3. Apply the following settingsTab Setting ValueColor Range User SpecifiedMin 0.2 [m s^-1]Max 2.2 [m s^-1] Note: Portions of streamlines that have values outside the range shown in the legend are colored according to the color at the nearest end of the legend. When using tubes or symbols (which contain faces), more accurate colors are obtained with lighting turned off. 4. Click Apply. The streamlines are colored using the specified range of velocity values.Coloring Streamlines with a Constant Color 1. Apply the following settingsTab Setting ValueColor ModeConstantColor (Green)ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 89Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.101. Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-Post Color can be set to green by selecting it from the color pallet, or by repeatedly clicking on the color box until it cycles through to the default green color. 2. Click Apply.Duplicating and Modifying a Streamline Object Any object can be duplicated to create a copy for modification without altering the original.Procedure1. Right-click MainStream and select Duplicate from the shortcut menu. 2. In the Name window, type SideStream. 3. Click OK. 4. Double click on the newly created streamline, SideStream. 5. Apply the following settings TabSetting Value Geometry Definition > Start From side inlet ColorModeConstantColor (Red) 6. Click Apply.Red streamlines appear, starting from the side inlet. 7. For better view, select Isometric View (Y up).Examining Turbulent Kinetic Energy A common way of viewing various quantities within the domain is to use a slice plane, as demonstrated in this module. Note: This module has multiple changes compiled into single steps in preparation for other tutorials that provide fewer specific instructions.Procedure1. Clear visibility for both the MainStream and the SideStream objects. 2. Create a plane named Plane 1 that is normal to X and passing through the X = 0 Point.To do so, specific instructions follow. a. From the main menu, select Insert > Location > Plane and click OK. b. In the Details view set Definition > Method to YZ Plane and X to 0 [m]. c. Click Apply. 3. Color the plane using the variable Turbulence Kinetic Energy, to show regions ofhigh turbulence. To do so, apply the settings below. TabSetting Value ColorModeVariableVariableTurbulence Kinetic Energy 4. Click Apply.Page 90 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.102. Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-Post 5. Experiment with other variables to color this plane (for example, Temperature to showthe temperature mixing of the two streams). Commonly used variables are in the drop-down menu. A full list of available variables can be viewed by clicking next to the Variable data box.Exiting ANSYS CFX-Post When finished with ANSYS CFX-Post exit the current window. Two procedures are documented. Depending on your installation of ANSYS CFX, follow either the Standalone procedure or the Workbench procedure.Procedure in 1. When you are finished, select File > Quit to exit ANSYS CFX-Post.Standalone 2. Click Quit if prompted to save.Procedure in 1. When you are finished, select File > Close to close the current file.Workbench2. Click Close if prompted to save. 3. Return to the Project page. Select File > Close Project. 4. Select No, then close Workbench.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 91Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.103. Tutorial 3: Flow in a Process Injection Mixing Pipe: Viewing the Results in ANSYS CFX-PostPage 92 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.104. Tutorial 4:Flow from a Circular VentIntroduction This tutorial includes: • Tutorial 4 Features (p. 94) • Overview of the Problem to Solve (p. 95) • Defining a Steady-State Simulation in ANSYS CFX-Pre (p. 95) • Obtaining a Solution to the Steady-State Problem (p. 99) • Defining a Transient Simulation in ANSYS CFX-Pre (p. 100) • Obtaining a Solution to the Transient Problem (p. 104) • Viewing the Results in ANSYS CFX-Post (p. 105) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 95). Sample files referenced by this tutorial include: • CircVent.pre • CircVentIni.pre • CircVentIni_001.res • CircVentMesh.gtm • CircVentIni.cfx • CircVentIni.gtmANSYS CFX TutorialsPage 93ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.105. Tutorial 4: Flow from a Circular Vent: Tutorial 4 FeaturesTutorial 4 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateTransientFluid TypeGeneral FluidDomain Type Single DomainTurbulence Modelk-EpsilonBoundary Conditions Inlet (Subsonic)OpeningWall: No-SlipTimestepAuto Time ScaleTransient ExampleTransient Results FileANSYS CFX-PostPlots AnimationIsosurfaceOther Auto AnnotationMPEG GenerationPrintingTime Step SelectionTitle/TextTransient Animation In this tutorial you will learn about: • Setting up a transient problem in ANSYS CFX-Pre. • Using an opening type boundary condition in ANSYS CFX-Pre. • Modeling smoke using additional variables in ANSYS CFX-Pre. • Visualizing a smoke plume using an Isosurface in ANSYS CFX-Post. • Creating an image for printing, and generating an MPEG file in ANSYS CFX-Post.Page 94 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.106. Tutorial 4: Flow from a Circular Vent: Overview of the Problem to SolveOverview of the Problem to Solve In this example, a chimney stack releases smoke which is dispersed into the atmosphere with an oncoming side wind. Unlike previous tutorials, which were steady-state, this example is time-dependent. Initially, no smoke is being released. In the second part of the tutorial, the chimney starts to release smoke and it shows how the plume of smoke above the chimney develops with time.smoke speed varyingfrom zero to 0.2 m/s wind speed 1 m/sr=10 mDefining a Steady-State Simulation in ANSYS CFX-Pre This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre for a steady-state simulation with no smoke being produced by the chimney. The results from this simulation will be used as the initial guess for the transient simulation.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: CircVentIni.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution to the Steady-State Problem (p. 99).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type CircVentIni. 6. Click Save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 95Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.107. Tutorial 4: Flow from a Circular Vent: Defining a Steady-State Simulation in ANSYS CFX-PreImporting the Mesh 1. Select File > Import Mesh. 2. From your working directory, select CircVentMesh.gtm. 3. Click Open. 4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View(Z up) from the shortcut menu.Creating an Additional Variable In this tutorial, an additional variable (non-reacting scalar component) will be used to model the dispersion of smoke from the vent. Note: While smoke is not required for the steady-state simulation, including it here prevents the user from having to set up timevalue interpolation in the transient simulation. 1. From the main menu, select Insert > Expressions, Functions and Variables >Additional Variable or click Additional Variable. 2. Under Name, type smoke. 3. Click OK. 4. Under Variable Type, select Volumetric. 5. Set Units to [kg m^-3]. 6. Click OK.Creating the Domain The fluid domain will be created that includes the additional variable.To Create a New1. Select Insert > Domain from the main menu, or click Domain , then set the name toDomainCircVent and click OK. 2. Apply the following settings TabSetting Value General OptionsFluids List Air at 25 CReference Pressure0 [atm] Fluid Models Heat Transfer > OptionNoneAdditional Variable Details > smoke (Selected)Additional Variable Details > smoke > (Selected)Kinematic DiffusivityAdditional Variable Details > smoke > 1.0E-5 [m^2 s^-1]Kinematic Diffusivity > KinematicDiffusivity 3. Click OK.Page 96 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.108. Tutorial 4: Flow from a Circular Vent: Defining a Steady-State Simulation in ANSYS CFX-PreCreating the Boundary Conditions This is an example of external flow, since fluid is flowing over an object and not through an enclosure such as a pipe network (which would be an example of internal flow). In such problems, some inlets will be made sufficiently large that they do not affect the CFD solution. However, the length scale values produced by the Default Intensity and AutoCompute Length Scale option for turbulence are based on inlet size. They are appropriate for internal flow problems and particularly, cylindrical pipes. In general, you need to set the turbulence intensity and length scale explicitly for large inlets in external flow problems. If you do not have a value for the length scale, you can use a length scale based on a typical length of the object, over which the fluid is flowing. In this case, you will choose a turbulence length scale which is one-tenth of the diameter of the vent. Note: The boundary marker vectors used to display boundary conditions (Inlets, Outlets, Openings) are normal to the boundary surface regardless of the actual direction specification. To plot vectors in the direction of flow, select Boundary Vector under the Plot Options tab for the inlet boundary condition and clear Show Inlet Markers on the Boundary Marker Options tab of Labels and Markers (accessible by clicking Label and Marker Visibility ). For parts of the boundary where the flow direction changes, or is unknown, an opening boundary condition can be used. An opening boundary condition allows flow to both enter and leave the fluid domain during the course of the solution.Inlet Boundary 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 2. Under Name, type Wind. 3. Click OK. 4. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Inlet LocationWindBoundary Details Mass and Momentum > OptionCart. Vel. Components Mass and Momentum > U 1 [m s^-1] Mass and Momentum > V 0 [m s^-1] Mass and Momentum > W 0 [m s^-1] Turbulence > Option Intensity and Length Scale Turbulence > Value0.05 Turbulence > Eddy Len. Scale0.25 [m] Additional Variables > smoke > Option Value Additional Variables > smoke > Value0 [kg m^-3] 5. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 97Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.109. Tutorial 4: Flow from a Circular Vent: Defining a Steady-State Simulation in ANSYS CFX-PreOpening 1. Select Insert > Boundary Condition from the main menu or click Boundary ConditionBoundary.2. Under Name, type Atmosphere.3. Click OK.4. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Opening LocationAtmosphereBoundary Details Mass and Momentum > OptionOpening Pres. and Dirn Mass and Momentum > Relative Pressure 0 [Pa] Flow Direction > Option Normal to Boundary Condition Turbulence > Option Intensity and Length Scale Turbulence > Value0.05 Turbulence > Eddy Len. Scale0.25 [m] Additional Variables > smoke > Option Value Additional Variables > smoke > Value0 [kg m^-3]5. Click OK.Inlet for the 1. Select Insert > Boundary Condition from the main menu or click Boundary ConditionVent.2. Under Name, type Vent.3. Click OK.4. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Inlet LocationVentBoundary Details Mass and Momentum > Normal Speed0.01 [m s^-1] Turbulence > Option Intensity and Eddy Viscosity Ratio Additional Variables > smoke > Option Value Additional Variables > smoke > Value0 [kg m^-3]5. Click OK.Setting Initial Values1. Click Global Initialization .2. Select Turbulence Eddy Dissipation.3. Click OK.Page 98ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.110. Tutorial 4: Flow from a Circular Vent: Obtaining a Solution to the Steady-State ProblemSetting Solver Control ANSYS CFX-Solver has the ability to calculate physical timestep size for steady-state problems. If you do not know the time step size to set for your problem, you can use the Auto Timescale option. 1. Click Solver Control . 2. Apply the following settingsTabSettingValueBasic Settings Convergence Control > Max. Iterations75 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settingsSetting ValueFile name CircVentIni.defQuit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file.Obtaining a Solution to the Steady-State Problem When ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, you can obtain a solution to the CFD problem by using the following procedure. 1. Click Start Run.The residual plots for six equations will appear: U - Mom, V - Mom, W - Mom, P - Mass,K-TurbKE and E-Diss.K (the three momentum conservation equations, the massconservation equation and equations for the turbulence kinetic energy and turbulenceeddy dissipation). The Momentum and Mass tab contains four of the plots and theother two are under Turbulence Quantities. The variable smoke is also plotted butregisters no values since it is not initialized. 2. Click No to close the completion message, since you do not need to view the results inANSYS CFX-Post. 3. If using Standalone Mode, quit ANSYS CFX-Solver Manager. You will now reload the simulation into ANSYS CFX-Pre to define the transient simulation.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 99Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.111. Tutorial 4: Flow from a Circular Vent: Defining a Transient Simulation in ANSYS CFX-PreDefining a Transient Simulation in ANSYS CFX-PreIn this part of the tutorial, you alter the simulation settings used for the steady-statecalculation to set up the model for the transient calculation in ANSYS CFX-Pre.Playing a Session FileIf you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulationautomatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre,then run the session file: CircVent.pre. After you have played the session file as describedin earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager(p. 87), proceed to Obtaining a Solution to the Transient Problem (p. 104).Opening the Existing Simulation1. Start ANSYS CFX-Pre.2. Select File > Open Simulation.3. If required, set the path location to the tutorial folder.4. Select the simulation file CircVentIni.cfx.5. Click Open.6. Select File > Save Simulation As.7. Change the name to CircVent.cfx.8. Click Save.Modifying the Simulation TypeIn this step you will make the problem transient. Later, you will set the concentration ofsmoke to rise exponentially with time, so it is necessary to ensure that the interval betweenthe timesteps is smaller at the beginning of the simulation than at the end.1. Click Simulation Type .2. Apply the following settingsTabSetting ValueBasic Settings Simulation Type > OptionTransient Simulation Type > Time Duration > 30 [s] Total Time Simulation Type > Time Steps >4*0.25, 2*0.5, 2*1.0, 13*2.0 [s] Timesteps*† Simulation Type > Initial Time > Time 0 [s] *.Do NOT click Enter Expression to enter lists of values. Enter the list without the units, then set the units in the drop-down list. †.This list specifies 4 timesteps of 0.25 [s], then 2 timesteps of 0.5 [s], etc.3. Click OK.Page 100 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.112. Tutorial 4: Flow from a Circular Vent: Defining a Transient Simulation in ANSYS CFX-PreModifying the Boundary Conditions The only boundary condition which needs altering is the Vent boundary condition. In the steady-state calculation, this boundary had a small amount of air flowing through it. In the transient calculation, more air passes through the vent and there is a time-dependent concentration of smoke in the air. This is initially zero, but builds up to a larger value. The smoke concentration will be specified using the CFX Expression Language.To Modify the1. In the Outline workspace, expand the tree to Simulation > CircVent > Vent.Vent Inlet 2. Right-click Vent and select Edit.BoundaryCondition3. Apply the following settingsTabSettingValueBoundary Details Mass and Momentum > Normal Speed 0.2 [m s^-1] Leave the Vent details view open for now. You are going to create an expression for smoke concentration. The concentration is zero for time t=0 and builds up to a maximum of 1 kg m^-3. 4. Create a new expression by selecting Insert > Expressions, Functions and Variables> Expression from the main menu. Set the name to TimeConstant. 5. Apply the following settingsNameDefinitionTimeConstant3 [s] 6. Click Apply to create the expression. 7. Create the following expressions with specific settings, remembering to click Applyafter each is defined.NameDefinitionFinalConcentration1 [kg m^-3]ExpFunction * FinalConcentration*abs(1-exp(-t/TimeConstant)) *.When entering this function, you can select most of the required items by right-clicking in the Definition window in the Expression details view instead of typing them. The names of the existing expressions are under the Expressions menu. The exp and abs functions are under Functions > CEL. The variable t is under Variables. Note: The abs function takes the modulus (or magnitude) of its argument. Even though the expression (1- exp (-t/TimeConstant)) can never be less than zero, the abs function is included to ensure that the numerical error in evaluating it near to zero will never make the expression evaluate to a negative number. Next you will visualize how the expressions have scheduled the concentration of smoke issued from the vent.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 101Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.113. Tutorial 4: Flow from a Circular Vent: Defining a Transient Simulation in ANSYS CFX-PrePlotting Smoke1. Double-click ExpFunction in the Expressions tree view.Concentration 2. Apply the following settingsTabSetting ValuePlot t (Selected) Start of Range0 [s] End of Range30 [s]3. Click Plot Expression. The button name then changes to Define Plot, as shown.As can be seen, the smoke concentration rises exponentially, and reaches 90% of its finalvalue at around 7 seconds.4. Click the Boundary: Vent tab. In the next step, you will apply the expression ExpFunction to the additional variable smoke as it applies to the boundary Vent.5. Apply the following settingsTabSetting ValueBoundary Details Additional Variables > smoke > Option Value Additional Variables > smoke > Value* ExpFunction *.Click Enter Expression to enter text.6. Click OK.Page 102 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.114. Tutorial 4: Flow from a Circular Vent: Defining a Transient Simulation in ANSYS CFX-PreInitialization Values The steady state solution that you have finished calculating is used to supply the initial values to the ANSYS CFX-Solver. You can leave all of the initialization data set to Automatic and the initial values will be read automatically from the initial values file. Therefore, there is no need to revisit the initialization tab.Modifying the Solver Control 1. Click Solver Control . 2. Set Convergence Control > Max. Coeff. Loops to 3. 3. Leave the other settings at their default values. 4. Click OK to set the solver control parameters.Output Control To allow results to be viewed at different timesteps, it is necessary to create transient results files at specified times. The transient results files do not have to contain all solution data. In this step, you will create minimal transient results files.To Create1. From the main menu, select Insert > Solver > Output Control.Minimal2. Click the Trn Results tab.TransientResults Files3. Click Add new item and then click OK to accept the default name for the object. This creates a new transient results object. Each object can result in the production of many transient results files. 4. Apply the following settings to Transient Results 1Setting ValueOptionSelected VariablesOutput Variables List*Pressure, Velocity, smokeOutput Frequency > Option Time ListOutput Frequency > Time List† 1, 2 , 3 [s] *.Click the ellipsis icon to select items if they do not appear in the drop-down list. Use the key to select multiple items. †.Do NOT click Enter Expressionto enter lists of values. Enter the list without the units, then set the units in the drop-down list. 5. Click Apply. 6. Create a second item with the default name Transient Results 2 and apply thefollowing settings to that itemSetting ValueOptionSelected VariablesOutput Variables List Pressure, Velocity, smokeANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 103Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.115. Tutorial 4: Flow from a Circular Vent: Obtaining a Solution to the Transient Problem Setting Value Output Frequency > Option Time Interval Output Frequency > Time Interval* 4 [s]*.A transient results file will be produced every 4 s (including 0 s) and at 1 s, 2 s and3 s. The files will contain no mesh and data for only the three selected variables. Thisreduces the size of the minimal results files. A full results file is always written at theend of the run. 7. Click OK.Writing the Solver (.def) File 1. Click Write Solver File . 2. Apply the following settings Setting Value File name CircVent.def Quit CFX–Pre *Select*.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a Solution to the Transient Problem In this tutorial the ANSYS CFX-Solver will read the initial values for the problem from a file. For details, see Initialization Values (p. 103). You need to specify the file name. Define Run will be displayed when the ANSYS CFX-Solver Manager launches. Definition File will already be set to the name of the definition file just written. Notice that the text output generated by the ANSYS CFX-Solver will be more than you have seen for steady-state problems. This is because each timestep consists of several inner (coefficient) iterations. At the end of each timestep, information about various quantities is printed to the text output area. The variable smoke is now plotted under the Additional Variables tab. 1. Under Initial Values File, click Browse. 2. Select CircVentIni_001.res, which is the results file of the steady-state problem withno smoke issuing from the chimney. If you have not run the first part of this tutorial, copyCircVentIni_001.res from the /examples/ directory to your workingdirectory. 3. Click Open. 4. Click Start Run. 5. You may see a notice that the mesh from the initial values file will be used. This mesh isthe same as in the definition file. Click OK to continue.Page 104ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.116. Tutorial 4: Flow from a Circular Vent: Viewing the Results in ANSYS CFX-Post ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long time depending on your system. Eventually a dialog box is displayed. 6. When ANSYS CFX-Solver has finished, click Yes to post-process the results. 7. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-Post In this tutorial, you will view the dispersion of smoke from the vent over time. When ANSYS CFX-Post is loaded, the results that are immediately available are those at the final timestep; in this case, at t = 30 s (this is nominally designated Final State).Creating an Isosurface An isosurface is a surface of constant value of a variable. For instance, it could be a surface consisting of all points where the velocity is 1 [m s^-1]. In this case, you are going to create an isosurface of smoke density (smoke is the additional variable that you specified earlier). 1. Right-click on a blank area in the viewer and select Predefined Camera > IsometricView (Z up).This ensures that the view is set to a position that is best suited to display the results. 2. From the main menu, select Insert > Location > Isosurface or under Location, clickIsosurface. 3. Click OK. 4. Apply the following settings Tab Setting Value GeometryVariablesmoke Value 0.005 [kg m^-3] 5. Click Apply. • A bumpy surface will be displayed, showing the smoke starting to emerge from the vent. • The surface is rough because the mesh is coarse. For a smoother surface, you would re-run the problem with a smaller mesh length scale. • The surface will be a constant color as the default settings on the Color tab were used. • When Color Mode is set to either Constant or Use Plot Variable for an isosurface, it appears as one color. 6. In Geometry, experiment by changing the Value so that you can see the shape of theplume more clearly.Zoom in and rotate the geometry, as required. 7. When you have finished, set the Value to 0.002 [kg m^-3]. 8. Right-click on a blank spot in the viewer and select Predefined Camera > IsometricView (Z up).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 105Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.117. Tutorial 4: Flow from a Circular Vent: Viewing the Results in ANSYS CFX-PostViewing the Results at Different TimestepsThe Timestep Selector shows the Time Step (outer loop) number, the Time Value(simulated time in seconds) and the Type of results file that was saved at that timestep. Youcan see that Partial results files were saved (as requested in ANSYS CFX-Pre) for all timestepsexcept for the last one.1. Click Timestep Selector.2. Load the results for a time value of 2 s by double-clicking the appropriate row in the Timestep Selector. After a short pause, the Current Timestep (located just below the title bar of the Timestep Selector) will be updated with the new timestep number.3. Load the time value of 4 s using the Timestep Selector. The smoke has now spread out even more, and is being carried by the wind.4. Double-click some more time values to see how the smoke plume grows with time.5. Finish by loading a time value of 1 s.Generating Output FilesYou can produce image output from ANSYS CFX-Post.Adding a titleFirst, you will add text to the viewer so that the printed output has a title.1. Select Insert > Text from the main menu or click Create text.2. Click OK.3. In the Text String box, enter the following text.Isosurface showing smoke concentration of 0.002 kg/m^3 afterNote: Further text will be added at a later stage to complete this title.4. Select Embed Auto Annotation.5. Set Type to Time Value. In the text line, note that has been added to the end. This is where the time value will be placed.6. Click Apply to create the title.7. Click the Location tab to modify the position of the title. The default settings for text objects center text at the top of the screen. To experiment with the position of the text, change the settings on the Location tab.8. Under Appearance, change Color Mode to User Specified and select a new color.9. Click Apply.JPEG output ANSYS CFX-Post can produce hard-copy output in several different forms. In the nextsection you will print in JPEG format.1. Ensure a time value of 1 s is loaded.2. Select File > Print, or click Print.3. Under Format select JPEG.Page 106 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.118. Tutorial 4: Flow from a Circular Vent: Viewing the Results in ANSYS CFX-Post 4. Click Browsenext to the File data box. 5. Browse to the directory where you want the file saved. 6. Enter a name for the JPEG file. 7. Click Save to set the file name and directory.This sets the path and name for the file. 8. To print to the file, click Print.To view the file or make a hard copy, use an application that supports JPEG files. 9. Clear the visibility of the text object to hide it.To Generate an You can generate an MPEG file to show the transient flow of the plume of smoke. ToMPEG Filegenerate an MPEG file, you use the Animation dialog box in the same way as in Tutorial 1. However, to animate the plume of smoke, you need to animate over several timesteps. Note: On the Advanced tab of Animation Options, there is a check box option called Save frames as image files. By selecting this option, the JPEG or PPM files used to encode each frame of the MPEG will persist after MPEG creation; otherwise, they are deleted. Setting Keyframes 1. Click Animation . 2. Ensure that Keyframe Animation is selected. 3. Position the geometry so that you will be able to see the plume of smoke. 4. In the Animation dialog box, click Newto create KeyFrameNo1. 5. Load the time value of 30 s using the Timestep Selector. 6. Click New in the Animation dialog box to create KeyframeNo2. Defining additional options During the production of a transient animation, various timesteps will be loaded and all objects will be updated to use the results from that timestep. Each frame of the animation must use one of the available timesteps. In Animation, Timestep can be set to Timestep Interpolation, TimeValue Interpolation or Sequential Interpolation. This setting affects which timestep is loaded for each frame. 1. Click More Animation Options to show more animation settings. 2. Click Options. 3. Apply the following settingsTab SettingValueOptions Transient Case*TimeValue Interpolation *.This causes each frame to use the transient file having the closest time value. 4. Click OK. 5. Single click KeyframeNo1, then set # of Frames to 27 and press .ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 107Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.119. Tutorial 4: Flow from a Circular Vent: Viewing the Results in ANSYS CFX-PostThe animation now contains a total of 29 frames (27 intermediate frames plus the twokeyframes).6. Select Save MPEG.7. Click Browse next to Save MPEG.8. Under File name, type CircVent.mpg.9. If required, set the path location to a different folder.10. Click Save.The MPEG file name (including path) is set. At this point, the animation has not yet beenproduced.11. Click To Beginning .12. Click Play the animation .•The MPEG will be created as the animation proceeds.•This will be slow, since a timestep must be loaded and objects must be created for each frame.•To view the MPEG file, you need to use a viewer that supports the MPEG format.13. When you have finished, quit ANSYS CFX-Post.Page 108 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.120. Tutorial 5:Flow Around a Blunt BodyIntroduction This tutorial includes: • Tutorial 5 Features (p. 109) • Overview of the Problem to Solve (p. 111) • Defining a Simulation in ANSYS CFX-Pre (p. 111) • Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 116) • Viewing the Results in ANSYS CFX-Post (p. 119) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 111). Sample files referenced by this tutorial include: • BluntBody.pre • BluntBodyDist.cse • BluntBodyMesh.gtmTutorial 5 Features This tutorial addresses the following features of ANSYS CFX.ANSYS CFX TutorialsPage 109ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.121. Tutorial 5: Flow Around a Blunt Body: Tutorial 5 Features Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeIdeal Gas Domain Type Single Domain Turbulence ModelShear Stress Transport Heat Transfer Isothermal Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Symmetry Plane Wall: No-Slip Wall: Free-Slip TimestepPhysical Time Scale ANSYS CFX-Solver ManagerParallel processing ANSYS CFX-PostPlots Default Locators Outline Plot (Wireframe) Sampling Plane Streamline Vector Volume Other Changing the Color Range Instancing Transformation Lighting Adjustment Symmetry Viewing the MeshIn this tutorial you will learn about:• Solving and post-processing a case where the geometry has been omitted on one sideof a symmetry plane.• Using free slip wall boundaries on the sides of and above the domain as a compromisebetween accurate flow modeling and computational grid size.• Accurately modeling the near-wall flow using Shear Stress Transport (SST) turbulencemodel.• Running the ANSYS CFX-Solver in parallel (optional).• Creating vector plots in ANSYS CFX-Post with uniform spacing between the vectors.• Creating a macro using power syntax in ANSYS CFX-Post.Page 110 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.122. Tutorial 5: Flow Around a Blunt Body: Overview of the Problem to SolveOverview of the Problem to Solve This example demonstrates external air flow over a generic vehicle body. Since both the geometry and the flow are symmetric about a vertical plane, only half of the geometry will be used to find the CFD solution. Figure 1 External Air Flow Over a Generic Vehicle Bodyair speed15.0 m/s1.44 m 5.2 mDefining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: BluntBody.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 116).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type BluntBody. 6. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 111Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.123. Tutorial 5: Flow Around a Blunt Body: Defining a Simulation in ANSYS CFX-PreSetting ValueFile name BluntBodyMesh.gtm3. Click Open.Creating the DomainThe flow in the domain is expected to be turbulent and approximately isothermal. TheShear Stress Transport (SST) turbulence model with automatic wall function treatment willbe used because of its highly accurate predictions of flow separation. To take advantage ofthe SST model, the boundary layer should be resolved with at least 10 mesh nodes. In orderto reduce computational time, the mesh in this tutorial is much coarser than that.This tutorial uses an ideal gas as the fluid whereas previous tutorials have used a specificfluid. When modeling a compressible flow using the ideal gas approximation to calculatedensity variations, it is important to set a realistic reference pressure. This is because somefluid properties depend on the absolute fluid pressure (calculated as the static pressure plusthe reference pressure).1. Click Domain, and set the name to BluntBody.2. Apply the following settings to BluntBody:Tab SettingValueGeneral Options Basic Settings > Fluids List Air Ideal GasDomain Models > Pressure > Reference Pressure1 [atm]Fluid ModelsHeat Transfer > Option IsothermalHeat Transfer > Fluid Temperature288 [K]Turbulence > OptionShear Stress Transport3. Click OK.Creating Composite RegionsAn imported mesh may contain many 2D regions. For the purpose of creating boundaryconditions, it can sometimes be useful to group several 2D regions together and apply asingle boundary condition to the composite 2D region. In this case, you are going to createa Union between two regions that both require a free slip wall boundary condition.1. From the main menu, select Insert > Composite Region.2. Set the name to FreeWalls and click OK.3. Apply the following settingsTab SettingValueBasic SettingsDimension (Filter) 2D4. In the region list, hold down the key and select Free1 and Free2.Page 112 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.124. Tutorial 5: Flow Around a Blunt Body: Defining a Simulation in ANSYS CFX-Pre 5. Click OK.Creating the Boundary Conditions The simulation requires inlet, outlet, wall (no slip and free slip) and symmetry plane boundary conditions. The regions for these boundary conditions were defined when the mesh was created (except for the composite region just created for the free slip wall boundary condition).Inlet Boundary 1. Click Boundary Condition. 2. Under Name, type Inlet. 3. Apply the following settingsTabSetting ValueBasic Settings Boundary TypeInlet LocationInletBoundary Details Flow Regime > Option Subsonic Mass and Momentum > Option Normal Speed Mass and Momentum > Normal Speed 15 [m s^-1] Turbulence > OptionIntensity and Length Scale Turbulence > Eddy Len. Scale 0.1 [m] 4. Click OK.Outlet 1. Create a new boundary condition named Outlet.Boundary 2. Apply the following settingsTabSetting ValueBasic Settings Boundary TypeOutlet LocationOutletBoundary Details Mass and Momentum > Option Static Pressure Mass and Momentum > Relative Pressure 0 [Pa] 3. Click OK.Free Slip Wall The top and side surfaces of the rectangular region will use free slip wall boundaryBoundary conditions. • On free slip walls the shear stress is set to zero so that the fluid is not retarded. • The velocity normal to the wall is also set to zero. • The velocity parallel to the wall is calculated during the solution. This is not an ideal boundary condition for this situation since the flow around the body will be affected by the close proximity to the walls. If this case was modeling a wind tunnel experiment, the domain should model the size and shape of the wind tunnel and use no-slip walls. If this case was modeling a blunt body open to the atmosphere, a much larger domain should be used to minimize the effect of the walls.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 113Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.125. Tutorial 5: Flow Around a Blunt Body: Defining a Simulation in ANSYS CFX-PreYou will apply a single boundary condition to both walls by using the composite regiondefined earlier.1. Create a new boundary condition named FreeWalls.2. Apply the following settings:TabSetting ValueBasic Settings Boundary Type Wall LocationFreeWallsBoundary Details Wall Influence On Flow > Option Free Slip3. Click OK.Symmetry Plane 1. Create a new boundary condition named SymP.Boundary 2. Apply the following settings:TabSetting ValueBasic Settings Boundary Type Symmetry LocationSymP3. Click OK.Wall Boundary 1. Create a new boundary condition named Body.on the Blunt2. Apply the following settings:Body SurfaceTabSetting ValueBasic Settings Boundary Type Wall LocationBodyBoundary Details Wall Influence On Flow > Option No Slip3. Click OK.The remaining 2D regions (in this case, just the low Z face) will be assigned the defaultboundary condition which is an adiabatic, no-slip wall condition. In this case, the name ofthe default boundary condition is Default Boundary. Although the boundary conditionsBody and Default Boundary are identical (except for their locations), the Body boundarycondition was created so that, during post-processing, its location can by convenientlydistinguished from the other adiabatic, no-slip wall surfaces.Setting Initial Values1. Click Global Initialization .2. Apply the following settings:Page 114 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.126. Tutorial 5: Flow Around a Blunt Body: Defining a Simulation in ANSYS CFX-PreTab Setting ValueGlobal Settings Initial Conditions > Cartesian Velocity Automatic with ValueComponents > OptionInitial Conditions > Cartesian Velocity 15 [m s^-1]Components > UInitial Conditions > Cartesian Velocity 0 [m s^-1]Components > VInitial Conditions > Cartesian Velocity 0 [m s^-1]Components > WInitial Conditions > Turbulence Eddy(Selected)Dissipation 3. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settings:TabSettingValueBasic Settings Convergence Control > Max. Iterations60 Convergence Control > Fluid Timescale Control >Physical Timescale Timescale Control Convergence Control > Fluid Timescale Control >2 [s] Physical Timescale Convergence Criteria > Residual Target 1e-05 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settings:Setting ValueFile name BluntBody.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 115Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.127. Tutorial 5: Flow Around a Blunt Body: Obtaining a Solution Using ANSYS CFX-Solver ManagerObtaining a Solution Using ANSYS CFX-Solver ManagerThis tutorial introduces the parallel solver capabilities of ANSYS CFX.Note: The results produced will be identical, whether produced by a parallel or serial run.If you do not want to solve this tutorial in parallel (on more than one processor) or you donot have a license to run the ANSYS CFX-Solver in parallel, proceed to Obtaining a Solutionin Serial (p. 116).If you do not know if you have a license to run the ANSYS CFX-Solver in parallel, you shouldeither ask your system administrator, or query the license server (see the ANSYS, Inc.Licensing Guide (which is installed with the ANSYS License Manager) for details).Alternatively proceed to Obtaining a Solution in Serial (p. 116).If you would like to solve this tutorial in parallel on the same machine, proceed to Obtaininga Solution with Local Parallel (p. 117).If you would like to solve this tutorial in parallel across different machines, proceed toObtaining a Solution with Distributed Parallel (p. 117).Obtaining a Solution in SerialWhen ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, you canobtain a solution to the CFD problem by using the following procedure.1. Click Start Run.2. Click Yes to process the results in ANSYS CFX-Post.3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Continue this tutorial from Viewing the Results in ANSYS CFX-Post (p. 119).Obtaining a Solution in ParallelBackground toUsing the parallel capability of the ANSYS CFX-Solver allows you to divide a large CFDParallel Running problem so that it can run on more than one processor/machine at once. This saves timein ANSYS CFX and, when multiple machines are used, avoids problems which arise when a CFD calculation requires more memory than a single machine has available. The partition (division) of the CFD problem is automatic.A number of events occur when you set up a parallel run and then ask the ANSYS CFX-Solverto calculate the solution:• Your mesh will be divided into the number of partitions that you have chosen.• The ANSYS CFX-Solver runs separately on each of the partitions on the selectedmachine(s).• The results that one ANSYS CFX-Solver process calculates affects the other ANSYSCFX-Solver processes at the interface between the different sections of the mesh.• All of the ANSYS CFX-Solver processes are required to communicate with each otherand this is handled by the master process.Page 116 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.128. Tutorial 5: Flow Around a Blunt Body: Obtaining a Solution Using ANSYS CFX-Solver Manager • The master process always runs on the machine that you are logged into when the parallel run starts. The other ANSYS CFX-Solver processes are slave processes and may be run on other machines. • After the problem has been solved, a single results file is written. It will be identical to a results file from the same problem run as a serial process, with one exception: an extra variable Real partition number will be available for the parallel run. This variable will be used later in this tutorial during post processing.Obtaining aTo run in local parallel mode, the machine you are on must have more than one processor.Solution with In ANSYS CFX-Solver Manager, the Define Run dialog box should already be open.Local Parallel 1. Leave Type of Run set to Full.If Type of Run was instead set to Partitioner Only, your mesh would be split into anumber of partitions but would not be run in the ANSYS CFX-Solver afterwards. 2. Set Run Mode to PVM Local Parallel .This is the recommended method for most applications. 3. If required, click Add Partitionto add more partitions.By default, 2 partitions are assigned. 4. Select Show Advanced Controls. 5. Click the Partitioner tab at the top of the dialog box. 6. Use the default MeTiS partitioner.Your model will be divided into two sections, with each section running in its ownANSYS CFX-Solver process. The default is the MeTiS partitioner because it producesmore efficient partitions than either Recursive Coordinate Bisection or UserSpecified Direction. 7. Click Start Run. 8. Click Post–Process Results. 9. If using ANSYS CFX-Solver in Standalone Mode, select Shut down Solver Manager, andthen click OK. Continue this tutorial from Text Output when Running in Parallel (p. 118).Obtaining aBefore running in Distributed Parallel mode, please ensure that your system has beenSolution withconfigured as described in the installation documentation.DistributedParallel In ANSYS CFX-Solver Manager, the Define Run dialog box should already be open. 1. Leave Type of Run set to Full.If Type of Run was instead set to Partitioner Only, your mesh would be split into anumber of partitions but would not be run in the ANSYS CFX-Solver afterwards. 2. Set Run Mode to PVM Distributed Parallel.The name of the machine that you are currently logged into should be in the HostName list. You are going to run with two partitions on two different machines, soanother machine must be added. 3. Click Insert Host to specify a new host machine.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 117Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.129. Tutorial 5: Flow Around a Blunt Body: Obtaining a Solution Using ANSYS CFX-Solver Manager•The Select Parallel Hosts dialog box is displayed. This is where you choose additional machines to run your processes.•Your system administrator should have set up a hosts file containing a list of the machines that are available to run the parallel ANSYS CFX-Solver.•The Host Name column displays names of available hosts.•The second column shows the number of processors on that machine.•The third shows the relative processor speed: a processor on a machine with a relative speed of 1 would typically be twice as fast as a machine with a relative speed of 0.5.•The last column displays operating system information.•This information is read from the hosts file; if any information is missing or incorrect your system administrator should correct the hosts file.Note: The # processors, relative speed and system information does not have to be specifiedto be able to run on a host.4. Select the name of another machine in the Host Name list. Select a machine that you can log into.5. Click Add. The name of the machine is added to the Host Name column.Note: Ensure that the machine that you are currently logged into is in the Hosts Name listin the Define Run dialog box.6. Close the Select Parallel Hosts dialog box.7. Select Show Advanced Controls.8. Click the Partitioner tab at the top of the dialog box.9. Use the default MeTiS partitioner. Your model will be divided into two sections, with each section running in its own ANSYS CFX-Solver process. The default is the MeTiS partitioner because it produces more efficient partitions than either Recursive Coordinate Bisection or User Specified Direction.10. Click Start Run to begin the parallel run.11. Click OK on the pop-up message.12. Click Yes to post-process the results when the completion message appears at the endof the run.13. Close ANSYS CFX-Solver Manager.Text Output The text output area shows what is being written to the output file. You will see informationwhen Runningsimilar to the following:in Parallel +--------------------------------------------------------------------+|Job Information |+--------------------------------------------------------------------+Run mode: partitioning runHost computer: fastmachine1Job started:Wed Nov 28 15:18:40 2005Page 118 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.130. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-Post This tells you that the information following is concerned with the partitioning. After the partitioning job has finished, you will find: CPU-Time requirements: - Preparations 1.460E+00 seconds - Low-level mesh partitioning1.000E-01 seconds - Global partitioning information3.100E-01 seconds - Vertex, element and face partitioning information 1.600E-01 seconds - Element and face set partitioning information5.000E-02 seconds - Summed CPU-time for mesh partitioning2.080E+00 seconds +--------------------------------------------------------------------+ | Job Information| +--------------------------------------------------------------------+ Host computer: fastmachine1 Job finished:Wed Nov 28 15:19:16 2005 Total CPU time: 1.143E+01 seconds or: (0: 0:0:11.428 ) ( Days: Hours:Minutes: Seconds ) This marks the end of the partitioning job. The ANSYS CFX-Solver now begins to solve your parallel run: +--------------------------------------------------------------------+ |Job Information | +--------------------------------------------------------------------+ Run mode: parallel run (PVM) Host computer: fastmachine1 Par. Process: Master running on mesh partition: 1 Job started:Thu Nov 28 15:19:20 2005 Host computer: slowermachine Par. Process: Slave running on mesh partition:2 Job started:Thu Nov 28 15:24:55 2005 The machine that you are logged into runs the master process, and controls the overall simulation. The second machine selected will run the slave process. If you had more than two processes, each additional process is run as a slave process. The master process in this example is running on the mesh partition number 1 and the slave is running on partition number 2. You can find out which nodes and elements are in each partition by using ANSYS CFX-Post later on in the tutorial. When the ANSYS CFX-Solver finishes, the output file displays the job information and a pop-up message to indicate completion of the run.Viewing the Results in ANSYS CFX-Post In this tutorial, a vector plot is created in ANSYS CFX-Post. This will let you see how the flow behaves around the body. You will also use symmetry planes and learn more about manipulating the geometry view in the viewer.Using Symmetry Planes Earlier in this tutorial you used a symmetry plane boundary condition because the entire blunt body is symmetrical about a plane. Due to this symmetry, it was necessary to use only half of the full geometry to calculate the CFD results. However, for visualization purposes, it is helpful to use the full blunt body. ANSYS CFX-Post is able to recreate the full data set from the half that was originally calculated. This is done by creating an Instance Transform object.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 119Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.131. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-PostManipulatingYou need to manipulate the geometry so that you will be able to see what happens whenthe Geometryyou use the symmetry plane. The ANSYS CFX-Post features that you have used in earliertutorials will not be described in detail. New features will be described in detail.1. Right-click a blank area in the viewer and select Predefined Camera > View Towards +X.Creating an Instance Transforms are used to visualize a full geometry representation in cases where theInstancesimulation took advantage of symmetry to solve for only part of the geometry. There areTransformthree types of transforms that you can use: Rotation, Translation, Reflection. In this tutorial,you will create a Reflection transform located on a plane.1. Click Location > Plane and set the name to Reflection Plane .2. Apply the following settings:Tab SettingValueGeometryDefinition > MethodZX PlaneRenderDraw Faces (cleared)3. Click Apply. This creates a plane in the same location as the symmetry plane defined in ANSYS CFX-Pre. Now the instance transform can be created using this Plane:4. From the main menu, select Insert > Instance Transform and accept the default name.5. Apply the following settings:Tab SettingValueDefinitionInstancing Info From Domain(Cleared)Apply Rotation (Cleared)Apply Reflection (Selected)Apply Reflection > Plane Reflection Plane6. Click Apply.Using the You can use the transform when creating or editing graphics objects. For example, you canReflectionmodify the Wireframe view to use it as follows:Transform1. Under the Outline tab, in User Locations and Plots, apply the following settings to Wireframe:TabSetting ValueView Apply Instancing Transform > TransformInstance Transform 12. Click Apply.3. Zoom so that the geometry fills the Viewer.You will see the full blunt body.Page 120 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.132. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-PostCreating Vectors You are now going to create a vector plot to show velocity vectors behind the blunt body. You need to first create an object to act as a locator, which, in this case, will be a sampling plane. Then, create the vector plot itself.Creating the A sampling plane is a plane with evenly spaced sampling points on it.Sampling Plane 1. Right-click a blank area in the viewer and select Predefined Camera > View Towards+Y.This ensures that the changes can be seen. 2. Create a new plane named Sample. 3. Apply the following settings:Tab Setting ValueGeometryDefinition > Method Point and NormalDefinition > Point6, -0.001, 1Definition > Normal 0, 1, 0Plane Bounds > Type RectangularPlane Bounds > X Size 2.5 [m]Plane Bounds > Y Size 2.5 [m]Plane TypeSamplePlane Type > X Samples20Plane Type > Y Samples20RenderDraw Faces(Cleared)Draw Lines(Selected) 4. Click Apply.You can zoom in on the sampling plane to see the location of the sampling points(where lines intersect). There are a total of 400 (20 * 20) sampling points on the plane. Avector can be created at each sampling point. 5. Hide the plane by clearing the visibility check box next to Sample.Creating a 1. Click Vectorand accept the default name.Vector Plot2. Apply the following settings:Using DifferentSamplingMethods Tab Setting ValueGeometryDefinition > LocationsSampleDefinition > Sampling VertexSymbolSymbol Size 0.25 3. Click Apply. 4. Zoom until the vector plot is roughly the same size as the viewer.You should be able to see a region of recirculation behind the blunt body.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 121Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.133. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-Post5. Ignore the vertices on the sampling plane and increase the density of the vectors by applying the following settings:TabSetting ValueGeometry Definition > Sampling Equally Spaced Definition > # of Points10006. Click Apply.7. Change the location of the Vector plot by applying the following setting:TabSetting ValueGeometry Definition > LocationsSymP8. Click Apply.Creating a Pressure Plot1. Apply the following settings to the boundary condition named Body:TabSetting ValueColorModeVariable VariablePressureView Apply Instancing Transform > TransformInstance Transform 12. Click Apply.3. Apply the following settings to SymP:TabSetting ValueRender Draw Faces(Cleared) Draw Line (Selected)4. Click Apply.You will be able to see the mesh around the blunt body, with the mesh length scaledecreasing near the body, but still coarse in the region of recirculation. By zooming in,you will be able to see the layers of inflated elements near the body.Creating Surface StreamlinesIn order to show the path of air along the surface of the blunt body, surface streamlines canbe made as follows:1. Clear the visibility of Body, SymP and Vector 1.2. Create a new plane named Starter.3. Apply the following settingsPage 122 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.134. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-PostTab Setting ValueGeometryDefinition > Method YZ PlaneX -0.1 [m] 4. Click Apply.The plane appears just upstream of the blunt body. 5. Clear the visibility check box for the plane.This hides the plane from view, although the plane still exists. 6. Click Streamline. and click OK to accept the default name. 7. Apply the following settings:Tab Setting ValueGeometryTypeSurface StreamlineDefinition > Surfaces BodyDefinition > Start From LocationsDefinition > LocationsStarterDefinition > Max Points 100Definition > DirectionForward 8. Apply the following settings. The surface streamlines appear on half of the surface of the blunt body. They start near the upstream end because the starting points were formed by projecting nodes from the plane to the blunt body.Moving Objects In ANSYS CFX-Post, you can reposition some locator objects directly in the viewer by using the mouse. 1. Select the visibility check box for the plane named Starter. 2. Select theSingle Select mouse pointer from the Selection Tools toolbar. 3. In the viewer, click the Starter plane to select it, then use the left mouse button to dragit along the X axis. Notice that the streamlines are redrawn as the plane moves.Creating a Surface Plot of y+ The velocity next to a no-slip wall boundary changes rapidly from a value of zero at the wall to the free stream value a short distance away from the wall. This layer of high velocity gradient is known as the boundary layer. Many meshes are not fine enough near a wall to accurately resolve the velocity profile in the boundary layer. Wall functions can be used in these cases to apply an assumed functional shape of the velocity profile. Other grids are fine enough that they do not require wall functions, and application of the latter has little effect.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 123Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.135. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-Post The majority of cases fall somewhere in between these two extremes, where the boundary layer is partially resolved by nodes near the wall and wall functions are used to supplement accuracy where the nodes are not sufficiently clustered near the wall. One indicator of the closeness of the first node to the wall is the dimensionless wall distance++y . It is good practice to examine the values of y at the end of your simulation. At the+ lower limit, a value of y less than or equal to 11 indicates that the first node is within the laminar sublayer of the boundary flow. Values larger than this indicate that an assumed logarithmic shape of the velocity profile is being used to model the boundary layer portion between the wall and the first node. Ideally you should confirm that there are several nodes (3 or more) resolving the boundary layer profile. If this is not observed, it is highly recommended that more nodes be added near the wall surfaces in order to improve simulation accuracy. In this tutorial, a coarse mesh is used to reduce the run time. Thus, the grid is far too coarse to resolve any of the boundary layer profile, and the solution is not highly accurate.Surface Plot ofA surface plot is one which colors a surface according to the values of a variable: in this case,y+++y . A surface plot of y can be obtained as follows: 1. Clear the visibility of all previous plots. 2. Under the Outline tab, apply the following settings to BluntBodyDefault: TabSetting Value ColorModeVariableVariableYplus* View Apply Instancing Transform > TransformInstance Transform 1*.Click the ellipsis icon to the right of the Variable dropdown menu to view a full listof variables, including Yplus. 3. Click Apply. 4. Under the Outline tab, apply the following settings to Body: TabSetting Value ColorModeVariableVariableYplus* View Apply Instancing Transform > TransformInstance Transform 1*.Click the ellipsis icon to the right of the Variable dropdown menu to view a full listof variables, including Yplus. 5. Click Apply.Page 124ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.136. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-PostDemonstrating Power Syntax This section demonstrates a power syntax macro used to evaluate the variation of any variable in the direction of the x-axis. This is an example of power syntax programming in ANSYS CFX-Post.Synopsis A macro containing CCL and power syntax will be loaded by playing a session file. This macro will be executed by entering a line of power syntax in the Command Editor dialog box. The macro tells ANSYS CFX-Post to create slice planes, normal to the X axis, at 20 evenly-spaced locations from the beginning to the end of the domain. On each plane, it measures and prints the minimum, maximum, and average values for a specified variable (using conservative values). The planes are colored using the specified variable. Note: The ANSYS CFX-Post engine can respond to CCL commands issued directly, or to commands issued using the graphical user interface. The Command Editor dialog box can be used to enter any valid CCL command directly.Procedure1. Play the session file named BluntBodyDist.cse. 2. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X. 3. Select Tools > Command Editor from the menu bar. 4. Type the following line into the Command Editor dialog box (the quotation marks andthe semi-colon are required): !BluntBodyDist("Velocity u"); 5. Click Process. The minimum, maximum and average values of the variable at each X location are written to the file BluntBody.txt. The results can be viewed by opening the file in a text editor. You can also run the macro with a different variable. To view the content of the session file (which contains explanatory comments), open the session file in a text editor. It contains all of the CCL and power syntax commands and will provide a better understanding of how the macro works.Viewing the Mesh Partitions (Parallel Only) If you solved this tutorial in parallel, then an additional variable named Real partition number will be available in ANSYS CFX-Post 1. Create an Isosurface of Real partition number equal to 1. 2. Create a second Isosurface of Real partition number equal to 1.999. The two Isosurfaces show the edges of the two partitions. The gap between the two plots shows the overlap nodes. These were contained in both partitions 1 and 2. When you have finished looking at the results, quit ANSYS CFX-Post.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 125Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.137. Tutorial 5: Flow Around a Blunt Body: Viewing the Results in ANSYS CFX-PostPage 126 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.138. Tutorial 6:Buoyant Flow in a PartitionedCavityIntroduction This tutorial includes: • Tutorial 6 Features (p. 128) • Overview of the Problem to Solve (p. 128) • Defining a Simulation in ANSYS CFX-Pre (p. 129) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 134) • Viewing the Results in ANSYS CFX-Post (p. 135) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 129). Sample files referenced by this tutorial include: • Buoyancy2D.geo • Buoyancy2D.preANSYS CFX TutorialsPage 127ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.139. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Tutorial 6 FeaturesTutorial 6 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type TransientFluid TypeGeneral FluidDomain Type Single DomainTurbulence ModelLaminarHeat Transfer Thermal EnergyBuoyant FlowBoundary Conditions Symmetry PlaneOutlet (Subsonic)Wall: No-SlipWall: AdiabaticWall: Fixed TemperatureOutput ControlTimestepTransient ExampleTransient Results FileANSYS CFX-PostPlots Default LocatorsReportOther Time Step SelectionTransient Animation In this tutorial you will learn about: • Using CFX-4 Mesh Import. • Setting up a time dependent (transient) simulation. • Modeling buoyant flow.Overview of the Problem to Solve This tutorial demonstrates the capability of ANSYS CFX in modeling buoyancy-driven flows which require the inclusion of gravitational effects.Page 128ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.140. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-Pre The model is a 2D partitioned cavity containing air. The bottom of the cavity is kept at a constant temperature of 75°C, while the top is held constant at 5°C. The cavity is also tilted at an angle of 30 degrees to the horizontal. A transient simulation is set up to see how the flow develops starting from stationary conditions. Since you are starting from stationary conditions, there is no need to solve a steady-state simulation for use as the initial guess. 5 C air75 C The mesh for the cavity was created in CFX-4 and has been provided.Defining a Simulation in ANSYS CFX-Pre You are going to import a hexahedral mesh originally generated in CFX-4. The mesh contains labelled regions which will enable you to apply the relevant boundary conditions for this problem.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: Buoyancy2D.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 134).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Create a new simulation using General Mode. 3. Select File > Save Simulation As and set File name to Buoyancy2D. 4. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. The Import Mesh dialog box appears.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 129Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.141. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-Pre2. Apply the following settingsSetting ValueFile type CFX-4File name Buoyancy2D.geo* *.This file is in your tutorial directory.3. Click Open.Simulation TypeThe default units and coordinate frame settings are suitable for this tutorial, but thesimulation type needs to be set to transient.You will notice physics validation messages as the case is set to Transient. These errors willbe fixed in the later part of the tutorial.1. Click Simulation Type .2. Apply the following settingsTabSetting ValueBasic Settings Simulation Type > OptionTransient Simulation Type > Time Duration > 2 [s] Total Time* Simulation Type > Time Steps >0.025 [s] Timesteps† Simulation Type > Initial Time > Time 0 [s] *.This is the total duration, in real time, for the simulation †.This is the interval from one step, in real time, to the next. The simulation will continue, moving forward in time by 0.025 s, until the total time has been reached3. Click OK.Page 130 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.142. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-PreCreating the Domain gsin3030 gcos30g y x30 You will model the cavity as if it were tilted at an angle of 30°. You can do this by specifying horizontal and vertical components of the gravity vector, which are aligned with the default coordinate axes, as shown in the diagram above.To Create a New1. Click Domain , and set the name to Buoyancy2D.Domain 2. Apply the following settings to Buoyancy2DTab Setting ValueGeneral Basic Settings > Fluids ListAir at 25 COptions Domain Models > Pressure > Reference Pressure 1 [atm]Domain Models > Buoyancy > Option BuoyantDomain Models > Buoyancy > Gravity X Dirn.-4.9 [m s^-2]Domain Models > Buoyancy > Gravity Y Dirn.-8.5 [m s^-2]Domain Models > Buoyancy > Gravity Z Dirn.0.0 [m s^-2]*Domain Models > Buoyancy > Buoy. Ref. Temp. 40 [C]†Fluid ModelsHeat Transfer > OptionThermal EnergyTurbulence > Option None (Laminar) *.This produces a gravity vector which simulates the tilt of the cavity †.Do not forget to change the units. This is just an approximate representative domain temperature. Initialization will be set up using Global Initialization, so there is no need to visit the Initialization tab. 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 131Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.143. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-PreCreating the Boundary ConditionsHot and ColdYou will create a wall boundary condition with a fixed temperature of 75 C on the bottomWall Boundary surface of the cavity, as follows:1. Create a new boundary condition named hot.2. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Wall LocationWALLHOTBoundary Heat Transfer > OptionTemperatureDetails Heat Transfer > Fixed Temperature 75 [C]3. Click OK.4. Create a new boundary condition named cold.5. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Wall LocationWALLCOLDBoundary Heat Transfer > OptionTemperatureDetailsHeat Transfer > Fixed Temperature 5 [C]6. Click OK.Symmetry Plane A single symmetry plane boundary condition can be used for the front and back of theBoundary cavity.1. Create a new boundary condition named SymP.2. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Symmetry LocationSYMMET1, SYMMET2* *.Use the key to select more than one region.3. Click OK.The default adiabatic wall boundary condition will automatically be applied to theremaining boundaries.Setting Initial ValuesYou should set initial settings using the Automatic with Value option when defining atransient simulation. Using this option, the first run will use the specified initial conditionswhile subsequent runs will use results file data for initial conditions.Page 132 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.144. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Defining a Simulation in ANSYS CFX-Pre 1. Click Global Initialization. 2. Apply the following settingsTabSettingValueGlobal SettingsInitial Conditions > Cartesian VelocityAutomatic with Components > OptionValue Initial Conditions > Cartesian Velocity0 [m s^-1] Components > U Initial Conditions > Cartesian Velocity0 [m s^-1] Components > V Initial Conditions > Cartesian Velocity0 [m s^-1] Components > W Initial Conditions > Static Pressure > Relative0 [Pa] Pressure Initial Conditions > Temperature > Temperature 5 [C] 3. Click OK.Setting Output Control 1. Click Output Control . 2. Click the Trn Results tab. 3. Create a new Transient Results item with the default name. 4. Apply the following settingsTabSetting ValueTrn ResultsTransient Results > Transient Results 1 > Selected Variables Option Transient Results > Transient Results 1 > Pressure, Temperature, Output Variables List*Velocity Transient Results > Transient Results 1 > Time Interval Output Frequency > Option Transient Results > Transient Results 1 > 0.1 [s] Output Frequency > Time Interval *.Click the ellipsis icon to select items if they do not appear in the drop-down list. Use the key to select multiple items. 5. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 133Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.145. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Obtaining a Solution using ANSYS CFX-Solver ManagerTab SettingValueBasic SettingsAdvection Scheme > OptionHigh ResolutionConvergence Control > Max. Coeff. Loops5Convergence Criteria > Residual Type RMSConvergence Criteria > Residual Target 1.E-4* *.An RMS value of at least 1.E-5 is usually required for adequate convergence, but the default value of 1.E-4 is sufficient for demonstration purposes.3. Click OK.Writing the Solver (.def) File1. Click Write Solver File .2. Apply the following settings:Setting ValueFile name Buoyancy2D.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode.3. Ensure Start Solver Manager is selected and click Save.4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a Solution using ANSYS CFX-Solver ManagerWhen ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, you canobtain a solution to the CFD problem by using the following procedure.Note: Recall that the output displayed on the Out File tab of the ANSYS CFX-Solver Manageris more complicated for transient problems than for steady-state problems. Each timestepconsists of several iterations, and after the timestep, information about various quantities isprinted.1. Click Start Run.2. Click Yes to post-process the results when the completion message appears at the end of the run.3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Page 134 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.146. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Viewing the Results in ANSYS CFX-PostViewing the Results in ANSYS CFX-Post In this section, you will create a report in ANSYS CFX-Post. You will also make an animation to see changes in temperature with time.Simple Report First, you will view a report that is created with little effort: 1. Click the Report Viewer tab. Note that the report loads with someautomatically-generated statistical information. 2. In the Outline tree view, under Report, experiment with the various settings for MeshReport, Physics Report and other report objects. These settings control the reportcontents. On the Report Viewer tab, you can click Refresh to see the changes to yourreport.Plots Here, you will create the following objects in preparation for generating a more customized report: • Contour plot of temperature • Point locators (for observing temperature) • Comment • Figure showing the contour plot and point locator • Time chart showing the temperature at the point locator • TableContour Plot 1. Click the 3D Viewer tab and right-click a blank area of the viewer, then selectPredefined Camera > View Towards -Z. 2. Select Insert > Contour from the main menu. 3. Accept the default name by clicking OK. 4. Set Locations to SymP. 5. Set Variable to Temperature. 6. Click Apply. The contour plot shows the temperature at the end of the simulation, since ANSYS CFX-Post loads values for the last timestep by default. You can load different timesteps using the Timestep Selector dialog box, accessible by selecting Tools > Timestep Selector from the main menu.Point Locators 1. From the main menu, select Insert > Location > Point. 2. Accept the default name by clicking OK. 3. Set Method to XYZ. 4. Set Point coordinates to 0.098, 0.05, 0.00125. 5. Click Apply.Note the location of Point 1 in the viewer.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 135Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.147. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Viewing the Results in ANSYS CFX-Post6. Right-click the Point 1 object in the tree view and select Duplicate from the shortcut menu.7. Accept the default name by clicking OK.8. Right-click the Point 2 object in the tree view and select Edit from the shortcut menu.9. Change the x-coordinate to 0.052.10. Click Apply.Note the location of Point 2 in the viewer.Comment 1. Click Create comment .2. Accept the default name by clicking OK. A comment object appears in the tree view, under the Report object.3. Set Heading to Buoyant Flow in a Partitioned Cavity.4. In the large text box, type:This is a sample paragraph.Figure1. Click the 3D Viewer tab.2. Select Insert > Figure from the main menu.3. Accept the default name by clicking OK. The Make copies of objects check box determines whether or not the objects that are visible in the viewer are copied. If objects are copied, then the copies are used in the figure instead of the originals. Since you are not using multiple views or figures, the check box setting does not matter.A figure object will appear under the Report branch in the tree view.Time Chart1. Select Insert > Chart from the main menu.2. Accept the default name by clicking OK.3. Set Title to Temperature versus Time.4. Set Type to Time.5. Click the Chart Line 1 tab.6. Set Line Name to Temperature at Point 1.7. Set Method to Point.8. Set Location to Point 1.9. Set Time Variable > Variable to Temperature.10. Click Apply.A chart object will appear under the Report branch in the tree view. The chart itself willappear in the Chart Viewer tab. It may take some time for the chart to appear becauseevery transient results file will be loaded in order to generate the time chart.11. Click New Line (on the Chart Line 1 tab).12. Set Line Name to Temperature at Point 2.13. Set Location to Point 2 and Time Variable > Variable to Temperature.14. Click Apply.A second chart line will appear in the chart, representing the temperature at Point 2.Table 1. Select Insert > Table from the main menu.Page 136 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.148. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Viewing the Results in ANSYS CFX-Post 2. Accept the default name by clicking OK.A table object will appear under the Report branch in the tree view. 3. Set the following:CellValueA1LocationA2Point 1A3Point 2B1TemperatureB2=probe(Temperature)@Point 1B3=probe(Temperature)@Point 2 The table shows temperatures at the end of the simulation, since ANSYS CFX-Post loads values for the last timestep by default. You can load different timesteps using the Timestep Selector dialog box, accessible by selecting Tools > Timestep Selector.Customized Report Right-click the Report object and select Refresh from the shortcut menu. Look at the report in the Report Viewer tab. Note that, in addition to the automatically-generated objects that you saw earlier when creating a simple report, this report also includes the customized figure, time chart and table described above.Animations Use the animation feature to see the changing temperature field. The animation feature was used in Tutorial 4: Flow from a Circular Vent (p. 93).Completion When you have finished, quit ANSYS CFX-Post.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 137Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.149. Tutorial 6: Buoyant Flow in a Partitioned Cavity: Viewing the Results in ANSYS CFX-PostPage 138 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.150. Tutorial 7:Free Surface Flow Over a BumpIntroduction This tutorial includes: • Tutorial 7 Features (p. 139) • Overview of the Problem to Solve (p. 140) • Defining a Simulation in ANSYS CFX-Pre (p. 141) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 148) • Viewing the Results in ANSYS CFX-Post (p. 149) • Using a Supercritical Outlet Condition (p. 154) If this is the first tutorial you are working with, it is important to review the following topics before beginning. • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 141). Sample files referenced by this tutorial include: • Bump2D.pre • Bump2DExpressions.ccl • Bump2Dpatran.outTutorial 7 Features This tutorial addresses the following features of ANSYS CFX:ANSYS CFX TutorialsPage 139ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.151. Tutorial 7: Free Surface Flow Over a Bump: Overview of the Problem to Solve Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeGeneral Fluid Domain Type Single Domain Turbulence Modelk-Epsilon Heat Transfer None Buoyant Flow Multiphase Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Symmetry Plane Wall: No-Slip Wall: Free-Slip CEL (CFX Expression Language) Mesh Adaption TimestepPhysical Time Scale ANSYS CFX-PostPlots Default Locators Isosurface Polyline Sampling Plane Vector Volume Other Chart Creation Title/Text Viewing the MeshIn this tutorial you will learn about:• Mesh import in PATRAN Neutral format.• Setting up a 2D problem.• Setting up appropriate boundary conditions for a free surface simulation. (Free surfacesimulations are more sensitive to incorrect boundary and initial guess settings thanother more basic models.)• Mesh adaption to refine the mesh where the volume fraction gradient is greatest. (Thisaids in the development of a sharp interface between the liquid and gas.)Overview of the Problem to SolveThis tutorial demonstrates the simulation of a free surface flow.The geometry consists of a 2D channel in which the bottom of the channel is interrupted bya semi-circular bump of radius 30 mm. The flow upstream of the bump is subcritical. Thedownstream conditions are not known but can be estimated using an analytical 1Dcalculation or data tables for flow over a bump.Page 140 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.152. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreDefining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: Bump2D.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 148).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type Bump2D. 6. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. The Import Mesh dialog box appears. 2. Apply the following settingsSetting ValueFile type PATRAN NeutralFile name Bump2Dpatran.out 3. Click Open. 4. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z from the shortcut menu.Viewing the1. Click Label and Marker Visibility .Region Labels2. Apply the following settingsTab SettingValueLabel Options Show Labels(Selected)Show Labels > Show Primitive3D Labels(Selected)Show Labels > Show Primitive2D Labels(Selected) 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 141Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.153. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreCreating Expressions for Initial and Boundary ConditionsSimulation of free surface flows usually requires defining boundary and initial conditions toset up appropriate pressure and volume fraction fields. You will need to create expressionsusing CEL (CFX Expression Language) to define these conditions.In this simulation, the following conditions are set and require expressions:• An inlet boundary where the volume fraction above the free surface is 1 for air and 0 forwater, and below the free surface is 0 for air and 1 for water.• A pressure-specified outlet boundary, where the pressure above the free surface isconstant and the pressure below the free surface is a hydrostatic distribution. Thisrequires you to know the approximate height of the fluid at the outlet. In this case, ananalytical solution for 1D flow over a bump was used. The simulation is not sensitive tothe exact outlet fluid height, so an approximation is sufficient. You will examine theeffect of the outlet boundary condition in the post-processing section and confirm thatit does not affect the validity of the results. It is necessary to specify such a boundarycondition to force the flow downstream of the bump into the supercritical regime.• An initial pressure field for the domain with a similar pressure distribution to that of theoutlet boundary.Either create expressions using the Expressions workspace or import expressions from afile.• Creating Expressions (p. 142)• Reading Expressions From a File (p. 143)Creating1. Right-click Expressions in the tree view and select Insert > Expression.Expressions 2. Set the name to UpH and click OK.3. Set Definition to 0.069 [m], and then click Apply.4. Use the same method to create the expressions listed in the table below. These are expressions for the downstream free surface height, the density of the fluid, the upstream volume fractions of air and water, the upstream pressure distribution, the downstream volume fractions of air and water, and the downstream pressure distribution.NameDefinitionDownH 0.022 [m]DenH998 [kg m^-3]UpVFAir step((y-UpH)/1[m])UpVFWater 1-UpVFAirUpPresDenH*g*UpVFWater*(UpH-y)DownVFAir step((y-DownH)/1[m])DownVFWater 1-DownVFAirDownPresDenH*g*DownVFWater*(DownH-y)5. Proceed to Creating the Domain (p. 143).Page 142 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.154. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreReading1. Copy the file Bump2DExpressions.ccl to your working directory from the ANSYS CFXExpressions examples directory.From a File2. Select File > Import CCL. 3. When Import CCL appears, ensure that Append is selected. 4. Select Bump2DExpressions.ccl. 5. Click Open. 6. After the file has been imported, use the Expression tree view to view the expressionsthat have been created.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settingsTab SettingValueGeneral Basic Settings > Fluids List Air at 25 C, WaterOptions Domain Models > Pressure > Reference Pressure1 [atm]Domain Models > Buoyancy > OptionBuoyantDomain Models > Buoyancy > Gravity X Dirn. 0 [m s^-2]Domain Models > Buoyancy > Gravity Y Dirn.*-gDomain Models > Buoyancy > Gravity Z Dirn. 0 [m s^-2]Domain Models > Buoyancy > Buoy. Ref. Density† 1.185 [kg m^-3]Domain Models > Buoyancy > Ref Location > Option AutomaticFluid ModelsMultiphase Options > Homogeneous Model‡(Selected)Multiphase Options > Free Surface Model > Option StandardHeat Transfer > Option IsothermalHeat Transfer > Fluid Temperature25 CTurbulence > Optionk-Epsilon *.You need to click Enter Expressionbeside the field first. †.Always set Buoyancy Reference Density to the density of the least dense fluid in free surface calculations. ‡.The homogeneous model solves for a single solution field. This is only appropriate in some simulations. 3. Click OK.Creating the Boundary ConditionsInlet Boundary 1. Create a new boundary condition named inflow. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 143Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.155. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic Boundary TypeInletSettingsLocation INFLOWBoundaryMass and Momentum > Option Normal SpeedDetailsMass and Momentum > Option > Normal Speed0.26 [m s^-1]Turbulence > OptionIntensity and Length ScaleTurbulence > Value 0.05Turbulence > Eddy Len. Scale*UpHFluid Values Boundary Conditions Air as 25 CAir at 25 C > Volume Fraction > Volume FractionUpVFAirBoundary ConditionsWaterWater > Volume Fraction > Volume FractionUpVFWater *.Click the Enter Expression icon.3. Click OK.Outlet1. Create a new boundary condition named outflow.Boundary2. Apply the following settingsTab SettingValueBasic Boundary TypeOutletSettingsLocation OUTFLOWBoundaryFlow Regime> OptionSubsonicDetails Mass and Momentum > Option Static PressureMass and Momentum > Relative PressureDownPres3. Click OK.Symmetry1. Create a new boundary condition named front.Boundary2. Apply the following settingsTab SettingValueBasic Boundary TypeSymmetrySettingsLocation FRONT3. Click OK.4. Create a new boundary condition named back.5. Apply the following settingsTab SettingValueBasic Boundary TypeSymmetrySettingsLocation BACKPage 144 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.156. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-Pre 6. Click OK.Wall and 1. Create a new boundary condition named top.Opening2. Apply the following settingsBoundariesTab SettingValueBasic SettingsBoundary TypeOpeningLocation TOPBoundary DetailsMass And Momentum > Option Static Pres. (Entrain)Mass And Momentum > Relative Pressure 0 [Pa]Turbulence > OptionZero GradientFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C >1.0Volume Fraction > Volume FractionBoundary ConditionsWaterBoundary Conditions > Water > Volume 0.0Fraction > Volume Fraction 3. Click OK. 4. Create a new boundary condition named bottom. 5. Apply the following settingsTabSetting ValueBasicBoundary Type WallSettings LocationBOTTOM1, BOTTOM2, BOTTOM3Boundary Wall Influence on Flow > Option No SlipDetailsWall Roughness > Option Smooth Wall 6. Click OK.Setting Initial Values 1. Click Global Initialization . 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 145Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.157. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreTab SettingValueGlobal Settings Initial Conditions > Cartesian VelocityAutomatic with ValueComponents > OptionInitial Conditions > Cartesian Velocity0.26 [m s^-1]Components > UInitial Conditions > Cartesian Velocity0 [m s^-1]Components > VInitial Conditions > Cartesian Velocity0 [m s^-1]Components > WInitial Conditions > Static Pressure > OptionAutomatic with ValueInitial Conditions > Static Pressure > RelativeUpPresPressureInitial Conditions > Turbulence Eddy Dissipation (Selected)Fluid SettingsFluid Specific Initialization > Air at 25 C(Selected)Air at 25 C > Initial Conditions > Volume Fraction > Automatic with ValueOptionAir at 25 C > Initial Conditions > Volume Fraction > UpVFAirVolume FractionFluid SettingsFluid Specific Initialization > Water(Selected)Fluid Specific Initialization > Water > InitialAutomatic with ValueConditions > Volume Fraction > OptionFluid Specific Initialization > Water > InitialUpVFWaterConditions > Volume Fraction > Volume Fraction3. Click OK.Setting Mesh Adaption Parameters1. Click Mesh Adaption .2. Apply the following settingsTabSetting ValueBasic Settings Activate Adaption (Selected) Save Intermediate Files (Cleared) Adaption Criteria > Variables ListAir at 25 C.Volume Fraction Adaption Criteria > Max. Num. Steps 2 Adaption Criteria > OptionMultiple of Initial Mesh Adaption Criteria > Node Factor 4 Adaption Convergence Criteria > Max.100 Iter. per StepAdvanced Options Node Alloc. Param.1.6 Number of Levels23. Click OK.Page 146 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.158. Tutorial 7: Free Surface Flow Over a Bump: Defining a Simulation in ANSYS CFX-PreSetting Solver Control Important: Setting Max Iterations to 200 and Number of Adaption Levels to 2 with a maximum of 100 timesteps each, results in a total maximum number of timesteps of 400 (2*100+200=400). 1. Click Solver Control . 2. Apply the following settingsTabSetting ValueBasic Settings Convergence Control > Max. Iterations 200 Convergence Control >Fluid TimescalePhysical Timescale Control > Timescale Control Convergence Control >Fluid Timescale0.25 [s] Control > Physical TimescaleAdvanced Options Multiphase Control(Selected) Multiphase Control > Volume Fraction(Selected) Coupling Multiphase Control > Volume FractionCoupled Coupling > Option Note: The options selected above activate the Coupled Volume Fraction solution algorithm. This algorithm typically converges better than the Segregated Volume Faction algorithm for buoyancy-driven problems such as this tutorial, which requires a 0.05 [s] timescale using the Segregated Volume Faction algorithm compared with 0.25 [s] for the Coupled Volume Fraction algorithm. Note: 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settings:Setting ValueFile name Bump2D.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 147Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.159. Tutorial 7: Free Surface Flow Over a Bump: Obtaining a Solution using ANSYS CFX-Solver ManagerObtaining a Solution using ANSYS CFX-Solver ManagerWhen ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, thesolution will be obtained.Within 100 iterations, the first adaption step will be performed. Information will be writtento the OUT file, containing the number of elements refined and the size of the new mesh.After mesh refinement, there will be a jump in the residual levels. This is because thesolution from the old mesh is interpolated on to the new mesh. A new residual plot will alsoappear for the W-Mom-Bulk equation. Hexahedral mesh elements are refined orthogonally,so the mesh is no longer 2D (it is more than 1 element thick in the z-direction). Y Before Refinement After Refinement X ZConvergence to the target residual level has been achieved. It is common for convergencein a residual sense to be difficult to obtain in a free surface simulation. This is due to thepresence of small waves at the surface preventing the residuals from dropping to the targetlevel. This is more frequently a problem in the subcritical flow regime, as the waves cantravel upstream. In the supercritical regime, the waves tend to get carried downstream andout the domain.To satisfy convergence in these cases, monitor the value of a global quantity, (for example,drag for flow around a ship’s hull) to see when a steady state value is reached.Where there is no obvious global quantity to monitor, you should view the results to seewhere the solution is changing. You can do this by running transient for a few timesteps,starting from a results file that you think is converged, or by writing some backup resultsfiles at different timesteps.In both cases look to see where the results are changing (this could be due to the presenceof small transient waves). Also confirm that the value of quantities that you are interested in(for example, downstream fluid height for this case) has reached a steady state value.1. Click Start Run.2. Click Yes to post-process the results when the completion message appears at the end of the run.3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Page 148 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.160. Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-PostViewing the Results in ANSYS CFX-Post 1. Select View Towards -Z by right-clicking on a blank area in the viewer and selectingPredefined Camera > View Towards -Z. 2. Zoom in so the geometry fills the Viewer. 3. In the tree view under Bump2D, edit front. 4. Apply the following settingsTabSettingValueColorMode Variable Variable Water.Volume Fraction 5. Click Apply. 6. Clear the check box next to front.Creating Velocity Vector Plots The next step involves creating a sampling plane to display velocity vectors for Water. 1. Create a new plane named Plane 1. 2. Apply the following settingsTabSettingValueGeometry Definition > MethodXY Plane Plane Bounds > TypeRectangular Plane Bounds > X Size1.25 [m] Plane Bounds > Y Size0.3 [m] Plane Bounds > X Angle 0 [degree] Plane Type Sample X Samples160 Y Samples40Render Draw Faces (Cleared) Draw Lines (Selected) 3. Click Apply. 4. Clear the check box next to Plane 1. 5. Create a new vector named Vector 1. 6. Apply the following settingsTabSettingValueGeometry Definition > Locations Plane 1 Definition > Variable* Water.VelocitySymbol Symbol Size0.5ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 149Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.161. Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-Post *.Since fluids in a free-surface calculation share the same velocity field, only the velocity of the first non-vapour fluid is available. The other allowed velocities are superficial velocities. For details, see Further Post-processing (p. 154).7. Click Apply.8. Apply the following settingsTab SettingValueGeometryDefinition > VariableAir at 25 C.Superficial VelocitySymbolSymbol Size0.15Normalize Symbols(Selected)9. Click Apply.Viewing Mesh RefinementIn this section, you will view the surface mesh on one of the symmetry boundaries, createvolume objects to show where the mesh was modified, and create a vector plot to visualizethe added mesh nodes.1. Clear the check box next to Vector 1..2. Zoom in so the geometry fills the Viewer.3. In Outline under Default Domain, edit front.4. Apply the following settingsTab SettingValueColor Mode ConstantRenderDraw Faces (Cleared)Draw Lines (Selected)5. Click Apply.•The mesh has been refined near the free surface.•In the transition region between different levels of refinement, tetrahedral and pyramidal elements are used since it is not possible to recreate hexahedral elements in ANSYS CFX. Near the inlet, the aspect ratio of these elements increases.Page 150 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.162. Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-Post •Avoid performing mesh refinement on high-aspect-ratio hex meshes, as this willproduce high aspect ratio tetrahedral-elements, resulting in poor mesh quality. Figure 1 Mesh around the bump 6. Create a new volume named first refinement elements. 7. Apply the following settings Tab SettingValue GeometryDefinition > MethodIsovolume Definition > VariableRefinement Level Definition > ModeAt Value Definition > Value 1 RenderDraw Faces (Cleared) Draw Lines (Selected) Draw Lines > Line Width2 Draw Lines > Color ModeUser Specified Draw Lines > Line Color(Green) 8. Click Apply.You will see a band of green which indicates the elements that include nodes addedduring the first mesh adaption. 9. Create a new volume named second refinement elements. 10. Apply the following settings Tab SettingValue GeometryDefinition > MethodIsovolume Definition > VariableRefinement Level Definition >Mode At Value Definition > Value 2 Color ColorWhiteANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 151Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.163. Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-PostTab SettingValueRenderDraw Faces (Selected)Draw Lines (Selected)Draw Lines > Line Width4Draw Lines > Color ModeUser SpecifiedDraw Lines > Line Color(Black)11. Click Apply.You will see a band of white (with black lines) which indicates the elements that includenodes added during the second mesh adaption.12. Zoom in to a region where the mesh has been refined.The Refinement Level variable holds an integer value at each node, which is either 0, 1or 2 (since you used a maximum of two adaption levels).The nodal values of refinement level will be visualized next.13. Create a new vector named Vector 2.14. Apply the following settingsTab SettingValueGeometryDefinition > LocationBump2DDefinition > Variable *(Any Vector Variable)Color Mode VariableVariable Refinement LevelSymbolSymbol CubeSymbol Size0.02Normalize Symbols(Selected) *.The variable’s magnitude and direction do not matter since you will change the vector symbol to a cube with a normalized size.15. Click Apply.Blue nodes (Refinement Level 0 according to the color legend) are part of the original mesh.Green nodes (Refinement Level 1) were added during the first adaption step. Red nodes(Refinement Level 2) were added during the second adaption step. Note that someelements contain combinations of blue, green, and red nodes.Creating a ChartNext, you will create a chart to show how the height of the free surface varies along thelength of the channel. To do this, you will need a Polyline which follows the free surface. Youcan create the Polyline from the intersecting line between one of the Symmetry planes andan Isosurface which shows the free surface. First you must create the Isosurface.1. Clear the visibility check boxes for all of the objects except Wireframe.2. Create a new isosurface named Isosurface 1.3. Apply the following settingsPage 152 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.164. Tutorial 7: Free Surface Flow Over a Bump: Viewing the Results in ANSYS CFX-PostTabSettingValueGeometry Definition > VariableWater.Volume Fraction Definition > Value 0.5 4. Click Apply.Creating isosurfaces using this method is a good way to visualize a free surface in a 3Dsimulation. 5. Right-click any blank area in the viewer, select Predefined Camera, then selectIsometric View (Y up).Creating a These steps explain creating a Polyline which follows the free surface:Polyline to 1. Clear the visibility check box for Isosurface 1.Follow the FreeSurface2. Create a new polyline named Polyline 1. 3. Apply the following settingsTabSettingValueGeometry Method Boundary Intersection Boundary Listfront Intersect With Isosurface 1 4. Click Apply. A green line is displayed that follows the high-Z edge of the isosurface.Creating a Chart 1. Create a new chart named Chart 1.to Show the The Chart Viewer tab is selected.Height of the 2. Apply the following settingsSurfaceTabSettingValueChart Line 1 Line Namefree surface height Location Polyline 1 X Axis > VariableX Y Axis > VariableY Appearance > Symbols RectangleChartTitleFree Surface Height for Flowover a Bump 3. Click Apply. As discussed in Creating Expressions for Initial and Boundary Conditions (p. 142), an approximate outlet elevation is imposed as part of the boundary condition, even though the flow is supercritical. The chart illustrates the effect of this, in that the water level rises just before the exit plane. It is evident from this plot that imposing the elevation does not affect the upstream flow.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 153Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.165. Tutorial 7: Free Surface Flow Over a Bump: Using a Supercritical Outlet ConditionThe chart shows a wiggle in the elevation of the free surface interface at the inlet. This isrelated to an overspecification of conditions at the inlet, since both the inlet velocity andelevation were specified. For a subcritical inlet, only the velocity or the total energy shouldbe specified. The wiggle is due to a small inconsistency between the specified elevation andthe elevation computed by the solver to obtain critical conditions at the bump. The wiggleis analogous to one found if pressure and velocity were both specified at a subsonic inlet, ina converging-diverging nozzle with choked flow at the throat.Further Post-processingYou may wish to create some plots using the .Superficial Velocity variables.This is the fluid volume fraction multiplied by the fluid velocity and is sometimes called thevolume flux. It is useful to use this variable for vector plots in separated multiphase flow, asyou will only see a vector where a significant amount of that phase exists.Using a Supercritical Outlet ConditionFor supercritical free surface flows, the supercritical outlet boundary condition is usually themost appropriate boundary condition for the outlet, since it does not rely on thespecification of the outlet pressure distribution (which depends on an estimate of the freesurface height at the outlet). The supercritical outlet boundary condition requires a relativepressure specification for the gas only; no pressure information is required for the liquid atthe outlet. For this tutorial, the relative gas pressure at the outlet should be set to 0 [Pa].The supercritical outlet condition may admit multiple solutions. To find the supercriticalsolution, it is often necessary to start with a static pressure outlet condition (as previouslydone in this tutorial) or an average static pressure condition where the pressure is setconsistent with an elevation to drive the solution into the supercritical regime. The outletcondition can then be changed to the supercritical option.Page 154 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.166. Tutorial 8:Supersonic Flow Over a WingIntroduction This tutorial includes: • Tutorial 8 Features (p. 155) • Overview of the Problem to Solve (p. 157) • Defining a Simulation in ANSYS CFX-Pre (p. 157) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 162) • Viewing the Results in ANSYS CFX-Post (p. 162) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 157). Sample files referenced by this tutorial include: • WingSPS.pre • WingSPSMesh.outTutorial 8 Features This tutorial addresses the following features of ANSYS CFX.ANSYS CFX TutorialsPage 155ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.167. Tutorial 8: Supersonic Flow Over a Wing: Tutorial 8 Features Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeIdeal Gas Domain Type Single Domain Turbulence ModelShear Stress Transport Heat Transfer Total Energy Boundary Conditions Inlet (Supersonic) Outlet (Supersonic) Symmetry Plane Wall: No-Slip Wall: Adiabatic Wall: Free-Slip Domain Interfaces Fluid-Fluid (No Frame Change) TimestepAuto Time Scale ANSYS CFX-PostPlots Contour Default Locators Vector Other Variable Details ViewIn this tutorial you will learn about:• Setting up a supersonic flow simulation.• Using the Shear Stress Transport turbulence model to accurately resolve flow aroundthe wing surface.• Defining custom vector variables for use in visualizing pressure distribution.Page 156 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.168. Tutorial 8: Supersonic Flow Over a Wing: Overview of the Problem to SolveOverview of the Problem to Solve This example demonstrates the use of ANSYS CFX in simulating supersonic flow over a symmetric NACA0012 airfoil at 0° angle of attack. A 2D section of the wing is modeled. A 2D hexahedral mesh is provided that is imported into ANSYS CFX-Pre. air speed 1.25 [m] u = 600 m/soutlet 30 [m]wing surface70 [m]Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: WingSPS.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 162).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type WingSPS. 6. Click Save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 157Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.169. Tutorial 8: Supersonic Flow Over a Wing: Defining a Simulation in ANSYS CFX-PreImporting the Mesh1. Right-click Mesh and select Import Mesh. The Import Mesh dialog box appears.2. Apply the following settingsSetting ValueFile type PATRAN NeutralFile name WingSPSMesh.out3. Click Open.4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Y up) from the shortcut menu.Creating the DomainCreating a New1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain Domain is selected. A domain named Default Domain should now appear under the Simulation branch.2. Double click it and apply the following settingsTabSetting ValueGeneral OptionsBasic Settings > Location WING Fluids List Air Ideal Gas Domain Models > Pressure >1 [atm] Reference Pressure*Fluid Models Heat Transfer > OptionTotal Energy† Turbulence > Option Shear Stress Transport *.When using an ideal gas, it is important to set an appropriate reference pressure since some properties depend on the absolute pressure level. †.The Total Energy model is appropriate for high speed flows since it includes kinetic energy effects.3. Click OK.Creating the Boundary ConditionsInlet Boundary1. Create a new boundary condition named Inlet.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation INLETPage 158 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.170. Tutorial 8: Supersonic Flow Over a Wing: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBoundary DetailsFlow Regime > OptionSupersonicMass and Momentum > OptionCart. Vel. & PressureMass and Momentum > U 600 [m s^-1]Mass and Momentum > V 0 [m s^-1]Mass and Momentum > W 0 [m s^-1]Mass and Momentum > Rel. Static Pres. 0 [Pa]Turbulence > Option Intensity and Length ScaleTurbulence > Value0.01Turbulence > Eddy Len. Scale0.02 [m]Heat Transfer > Static Temperature300 [K] 3. Click OK.Outlet 1. Create a new boundary condition named Outlet.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type OutletLocationOUTLETBoundary DetailsFlow Regime > OptionSupersonic 3. Click OK.Symmetry Plane 1. Create a new boundary condition named SymP1.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type SymmetryLocationSIDE1 3. Click OK. 4. Create a new boundary condition named SymP2. 5. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type SymmetryLocationSIDE2 6. Click OK. 7. Create a new boundary condition named Bottom. 8. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 159Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.171. Tutorial 8: Supersonic Flow Over a Wing: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic SettingsBoundary TypeSymmetryLocation BOTTOM9. Click OK.Free Slip 1. Create a new boundary condition named Top.Boundary2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeWallLocation TOPBoundary DetailsWall Influence on Flow > OptionFree Slip3. Click OK.Wall Boundary 1. Create a new boundary condition named WingSurface.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeWallLocation WING_Nodes* *.Click the ellipsisicon to select items if they do not appear in the drop-down list.3. Click OK.Creating Domain InterfacesThe imported mesh contains three regions which will be connected with domain interfaces.1. Create a new domain interface named Domain Interface 1.2. Apply the following settingsTabSetting ValueBasic Settings Interface TypeFluid Fluid Interface Side 1 > Region ListPrimitive 2D A* Interface Side 2 > Region ListPrimitive 2D, Primitive 2D B *.Click the ellipsisicon to select items if they do not appear in the drop-down list.3. Click OK.Page 160 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.172. Tutorial 8: Supersonic Flow Over a Wing: Defining a Simulation in ANSYS CFX-PreSetting Initial Values For high speed compressible flow, the ANSYS CFX-Solver usually requires sensible initial conditions to be set for the velocity field. 1. Click Global Initialization . 2. Apply the following settingsTab Setting ValueGlobalInitial Conditions > Cartesian Velocity Components > Option AutomaticSettingswith ValueInitial Conditions > Cartesian Velocity Components > U600 [m s^-1]Initial Conditions > Cartesian Velocity Components > V0 [m s^-1]Initial Conditions > Cartesian Velocity Components > W0 [m s^-1]Initial Conditions > Temperature > Option Automaticwith ValueInitial Conditions > Temperature > Temperature300 [K]Initial Conditions > Turbulence Eddy Dissipation(Selected) 3. Click OK.Setting Solver Control The residence time for the fluid is approximately: 70 [m] / 600 [m s^-1] = 0.117 [s] In the next step, you will start with a conservative time scale that gradually increases towards the fluid residence time as the residuals decrease. A user specified maximum time scale can be combined with an auto timescale in ANSYS CFX-Pre. 1. Click Solver Control . 2. Apply the following settingsTab SettingValueBasic SettingsConvergence Control > Fluid Timescale(Selected)Control > Maximum TimescaleConvergence Control > Fluid Timescale0.1 [s]Control > Maximum Timescale > MaximumTimescaleConvergence Criteria > Residual Target 1.0e-05 3. Click OK.Writing the Solver (.def) File Since this tutorial uses domain interfaces and the Summarize Interface Data toggle was selected, an information window is displayed that informs you of the connection type used for each domain interface.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 161Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.173. Tutorial 8: Supersonic Flow Over a Wing: Obtaining a Solution using ANSYS CFX-Solver Manager1. Click Write Solver File .2. Apply the following settingsSettingValueFile nameWingSPS.defSummarize Interface Data (Selected)Quit CFX–Pre*(Selected) *.If using ANSYS CFX-Pre in Standalone Mode.3. Ensure Start Solver Manager is selected and click Save.4. The Interface Summary dialog box is displayed. This displays information related to the summary of interface connections. Click OK.5. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a Solution using ANSYS CFX-Solver ManagerWhen ANSYS CFX-Pre has shut down, and the ANSYS CFX-Solver Manager has started,obtain a solution to the CFD problem by following the instructions below.1. In the ANSYS CFX-Solver Manager, click Start Run.2. Click Yes to post-process the results when the completion message appears at the end of the run.3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-PostThe following topics will be discussed:• Displaying Mach Information (p. 162)• Displaying Pressure Information (p. 163)• Displaying Temperature Information (p. 163)• Displaying Pressure With User Vectors (p. 163)Displaying Mach InformationThe first view configured shows that the bulk of the flow over the wing has a Mach Numberof over 1.5.1. Select View Towards -Z by typing +.2. Zoom in so the geometry fills the Viewer.3. Create a new contour named SymP2Mach.4. Apply the following settingsPage 162 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.174. Tutorial 8: Supersonic Flow Over a Wing: Viewing the Results in ANSYS CFX-PostTab Setting ValueGeometryLocations SymP2VariableMach NumberRange User SpecifiedMin 1Max 2# of Contours 21 5. Click Apply. 6. Clear the check box next to SymP2Mach.Displaying Pressure Information You will now create a contour plot that shows the pressure field. 1. Create a new contour named SymP2Pressure. 2. Apply the following settingsTab Setting ValueGeometryLocations SymP2VariablePressureRange Global 3. Click Apply. 4. Clear the check box next to SymP2Pressure.Displaying Temperature Information You can confirm that a significant energy loss occurs around the wing leading edge by plotting temperature on SymP2. The temperature at the wing tip is approximately 180 K higher than the inlet temperature. 1. Create a new contour named SymP2Temperature. 2. Apply the following settingsTab Setting ValueGeometryLocations SymP2VariableTemperatureRange Global 3. Click Apply. 4. Clear the check box next to SymP2Temperature.Displaying Pressure With User Vectors You can also try creating a user vector to show the pressure acting on the wing:ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 163Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.175. Tutorial 8: Supersonic Flow Over a Wing: Viewing the Results in ANSYS CFX-Post1. Create a new variable named Variable 1.2. Apply the following settingsName Setting ValueVariable 1 Vector(Selected) X Expression(Pressure+101325[Pa])*Normal X Y Expression(Pressure+101325[Pa])*Normal Y Z Expression(Pressure+101325[Pa])*Normal Z3. Click Apply.4. Create a new vector named Vector 1.5. Apply the following settingsTabSetting ValueGeometry Locations WingSurface VariableVariable 1Symbol Symbol Size 0.046. Click Apply.7. Zoom in on the wing in order to see the created vector plot.Page 164 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.176. Tutorial 9:Flow Through a Butterfly ValveIntroduction This tutorial includes: • Tutorial 9 Features (p. 165) • Overview of the Problem to Solve (p. 166) • Defining a Simulation in ANSYS CFX-Pre (p. 167) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 180) • Viewing the Results in ANSYS CFX-Post (p. 180) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 167). Sample files referenced by this tutorial include: • PipeValve.pre • PipeValve_inlet.F • PipeValveMesh.gtm • PipeValveUserF.preTutorial 9 Features This tutorial addresses the following features of ANSYS CFX.ANSYS CFX TutorialsPage 165ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.177. Tutorial 9: Flow Through a Butterfly Valve: Overview of the Problem to Solve Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeGeneral Fluid Domain Type Single Domain Turbulence Modelk-Epsilon Heat Transfer None Particle Tracking Boundary Conditions Inlet (Profile) Inlet (Subsonic) Outlet (Subsonic) Symmetry Plane Wall: No-Slip Wall: Rough CEL (CFX Expression Language) User Fortran TimestepAuto Time Scale ANSYS CFX-Solver ManagerPower-Syntax ANSYS CFX-PostPlots Animation Default Locators Particle Track Point Slice Plane Other Changing the Color Range MPEG Generation Particle Track Animation Quantitative Calculation SymmetryIn this tutorial you will learn about:• using a rough wall boundary condition in ANSYS CFX-Pre to simulate the pipe wall• creating a fully developed inlet velocity profile using either the CFX ExpressionLanguage or a User CEL Function• setting up a Particle Tracking simulation in ANSYS CFX-Pre to trace sand particles• animating particle tracks in ANSYS CFX-Post to trace sand particles through the domain• quantitative calculation of average static pressure in ANSYS CFX-Post on the outletboundaryOverview of the Problem to SolveIn industry, pumps and compressors are commonplace. An estimate of the pumpingrequirement can be calculated based on the height difference between source anddestination and head loss estimates for the pipe and any obstructions/joints along the way.Page 166 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.178. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre Investigating the detailed flow pattern around a valve or joint however, can lead to a better understanding of why these losses occur. Improvements in valve/joint design can be simulated using CFD, and implemented to reduce pumping requirement and cost. Max. Vel. 5 m/s r = 20 mm 288 K Valve Plate Flows can also contain particulates that affect the flow and cause erosion to pipe and valve components. The particle tracking capability of ANSYS CFX can be used to simulate these effects. In this example, water flows through a 20 mm radius pipe with a rough internal surface. The equivalent sand grain roughness is 0.2 mm. The flow is controlled by a butterfly valve, which is set at an angle of 55° to the vertical axis. The velocity profile is assumed to be fully developed at the pipe inlet. The flow contains sand particles ranging in size from 50 to 500 microns.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run one of the following session files available for this tutorial: • PipeValve.pre sets the inlet velocity profile using a CEL (ANSYS CFX Expression Language) expression. • PipeValveUserF.pre sets the inlet velocity profile using a User CEL Function that is defined by a Fortran subroutine. This session file requires that you have the required Fortran compiler installed and set in your system path. For details on which Fortran compiler is required for your platform, see the applicable ANSYS, Inc. installation guide. If you are not sure which Fortran compiler is installed on your system, try running the cfx5mkext command (found in /bin) from the command line and read the output messages.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 167Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.179. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreIf you choose to run a session file do so using the procedure described in earlier tutorialsunder Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), and thenproceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 180) once thesimulation setup is complete.Creating a New Simulation1. Start ANSYS CFX-Pre.2. Select File > New Simulation.3. Select General and click OK.4. Select File > Save Simulation As.5. Under File name, type PipeValve.6. Click Save.Importing the Mesh1. Right-click Mesh and select Import Mesh.2. Apply the following settingsSetting ValueFile name PipeValveMesh.gtm3. Click Open.Defining the Properties of SandThe material properties of the sand particles used in the simulation need to be defined. Heattransfer and radiation modeling are not used in this simulation, so the only property thatneeds to be defined is the density of the sand.To calculate the effect of the particles on the continuous fluid, between 100 and 1000particles are usually required. However, if accurate information about the particle volumefraction or local forces on wall boundaries is required, then a much larger number ofparticles needs to be modeled.When you create the domain, choose either full coupling or one-way coupling between theparticle and continuous phase. Full coupling is needed to predict the effect of the particleson the continuous phase flow field but has a higher CPU cost than one-way coupling.One-way coupling simply predicts the particle paths during post-processing based on theflow field, but without affecting the flow field.To optimise CPU usage, you can create two sets of identical particles. The first set will be fullycoupled and between 100 and 1000 particles will be used. This allows the particles toinfluence the flow field. The second set will use one-way coupling but a much highernumber of particles will be used. This provides a more accurate calculation of the particlevolume fraction and local forces on walls.1. Click Material then create a new material named Sand Fully Coupled.Page 168 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.180. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre 2. Apply the following settings:TabSetting ValueBasic Settings Material GroupParticle Solids Thermodynamic State (Selected)Material PropertiesThermodynamic Properties > Equation of2300 [kg m^-3] State > Density Thermodynamic Properties >Specific Heat (Selected) Capacity Thermodynamic Properties >Specific Heat 0 [J kg^-1 K^-1]* Capacity > Specific Heat Capacity Thermodynamic Properties > Reference(Selected) State Thermodynamic Properties > ReferenceSpecified Point State > Option Thermodynamic Properties > Reference300 [K] State > Ref. Temperature *.This value is not used because heat transfer is not modeled in this tutorial. 3. Click OK. 4. Under Materials, right-click Sand Fully Coupled and select Duplicate from theshortcut menu. 5. Name the duplicate Sand One Way Coupled. 6. Click OK. Sand One Way Coupled is created with properties identical to Sand Fully Coupled.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settingsTab SettingValueGeneral Options Basic Settings > Fluids List WaterBasic Settings > Particle Tracking (Selected)Basic Settings > Particle Tracking > Particles List Sand Fully Coupled,Sand One Way CoupledDomain Models > Pressure > Reference Pressure 1 [atm]Fluid ModelsHeat Transfer > Option NoneTurbulence > Optionk-Epsilon*ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 169Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.181. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreTab SettingValueFluid Details Sand Fully Coupled (Selected)Sand Fully Coupled > Morphology > Option Solid ParticlesSand Fully Coupled > Morphology > Particle (Selected)Diameter DistributionSand Fully Coupled > Morphology > Particle Normal in Diameter byDiameter Distribution > Option MassSand Fully Coupled > Morphology > Particle 50e-6 [m]Diameter Distribution > Minimum DiameterSand Fully Coupled > Morphology > Particle 500e-6 [m]Diameter Distribution > Maximum DiameterSand Fully Coupled > Morphology > Particle 250e-6 [m]Diameter Distribution > Mean DiameterSand Fully Coupled > Morphology > Particle 70e-6 [m]Diameter Distribution > Std. DeviationSand Fully Coupled > Erosion Model (Selected)Sand Fully Coupled > Erosion Model > OptionFinnieSand Fully Coupled > Erosion Model > Vel.2.0Power FactorSand Fully Coupled > Erosion Model > Reference 1 [m s^-1]Velocity *.The turbulence model only applies to the continuous phase and not the particle phases.3. Apply the following settingsPage 170 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.182. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreTab SettingValueFluid Details Sand One Way Coupled (Selected)Sand One Way Coupled > Morphology >Solid ParticlesOptionSand One Way Coupled > Morphology >(Selected)Particle Diameter DistributionSand One Way Coupled > Morphology >Normal in Diameter by MassParticle Diameter Distribution > OptionSand One Way Coupled > Morphology >50e-6 [m]Particle Diameter Distribution > MinimumDiameterSand One Way Coupled > Morphology >500e-6 [m]Particle Diameter Distribution > MaximumDiameterSand One Way Coupled > Morphology >250e-6 [m]Particle Diameter Distribution > MeanDiameterSand One Way Coupled > Morphology >70e-6 [m]Particle Diameter Distribution > Std.DeviationSand One Way Coupled > Erosion Model (Selected)Sand One Way Coupled > Erosion Model > FinnieOptionSand One Way Coupled > Erosion Model > 2.0Vel. Power FactorSand One Way Coupled > Erosion Model > 1 [m s^-1]Reference Velocity 4. Apply the following settingsTab SettingValueFluid Details Water(Selected)Water > Morphology > OptionContinuous FluidFluid Pairs Fluid PairsWater | Sand Fully CoupledFluid Pairs > Water | Sand Fully Coupled > Fully CoupledParticle CouplingFluid Pairs > Water | Sand Fully Coupled > Schiller NaumannMomentum Transfer > Drag Force > OptionFluid PairsWater | Sand One Way CoupledFluid Pairs > Water | Sand One Way Coupled > One-way CouplingParticle CouplingFluid Pairs > Water | Sand One Way Coupled > Schiller NaumannMomentum Transfer > Drag Force > Option 5. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 171Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.183. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreCreating the Inlet Velocity ProfileIn previous tutorials you have often defined a uniform velocity profile at an inlet boundary.This means that the inlet velocity near to the walls is the same as that at the center of theinlet. If you look at the results from these simulations, you will see that downstream of theinlet, a boundary layer will develop, so that the downstream near wall velocity is much lowerthan the inlet near wall velocity.You can simulate an inlet more accurately by defining an inlet velocity profile, so that theboundary layer is already fully developed at the inlet. The one seventh power law will beused in this tutorial to describe the profile at the pipe inlet. The equation for this is: 1 --r 7 U = W max ⎛ 1 – ---------- ⎞-(Eqn. 1) ⎝ R max⎠where W max is the pipe centerline velocity, R max is the pipe radius, and r is the distancefrom the pipe centerline.A non uniform (profile) boundary condition can be created by:• Creating an expression using CEL that describes the inlet profile.OR• Creating a User CEL Function which uses a user subroutine (linked to the ANSYSCFX-Solver during execution) to describe the inlet profile.OR• Loading a BC profile file (a file which contains profile data).Profiles created from data files are not used in this tutorial, but are used in the tutorialTutorial 3: Flow in a Process Injection Mixing Pipe (p. 77).In this tutorial, you use one of the first two methods listed above to define the velocityprofile for the inlet boundary condition. The results from each method will be identical.Using a CEL expression is the easiest way to create the profile. The User CEL Functionmethod is more complex but is provided as an example of how to use this feature. For morecomplex profiles, it may be necessary to use a User CEL Function or a BC profile file.To use the User CEL Function method, continue with this tutorial from User CEL FunctionMethod for the Inlet Velocity Profile (p. 173). Note that you will need access to a Fortrancompiler to be able to complete the tutorial by the User CEL Function method.To use the expression method, continue with the tutorial from this point.Expression1. Create the following expressions.Method for theInlet VelocityProfile NameDefinitionRmax20 [mm]Wmax5 [m s^-1]Wprof Wmax*(abs(1-r/Rmax)^0.143)Page 172 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.184. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre In the definition of Wprof, the variable r (radius) is a ANSYS CFX System Variable defined as:2 2 r =x +y(Eqn. 2) In this equation, x and y are defined as directions 1 and 2 (X and Y for Cartesian coordinate frames) respectively, in the selected reference coordinate frame. You should now continue with the tutorial from Creating the Boundary Conditions (p. 175).User CEL The Fortran subroutine has already been written for this tutorial.FunctionMethod for the Important: You must have the required Fortran compiler installed and set in your systemInlet Velocity path in order to run this part of the tutorial. If you do not have a Fortran compiler, you shouldProfileuse the expression method for defining the inlet velocity, as described in Expression Method for the Inlet Velocity Profile (p. 172). For details on which Fortran compiler is required for your platform, see the applicable ANSYS, Inc. installation guide. If you are not sure which Fortran compiler is installed on your system, try running the cfx5mkext command (found in /bin) from the command line and read the output messages. Compiling the Subroutine 1. Copy the subroutine PipeValve_inlet.F to your working directory. It is located in the/examples/ directory. 2. Examine the contents of this file in any text editor to gain a better understanding of thissubroutine.This file was created by modifying the ucf_template.F file, which is available in the/examples/ directory.You can compile the subroutine and create the required library files used by the ANSYSCFX-Solver at any time before running the ANSYS CFX-Solver. The operation isperformed at this point in the tutorial so that you have a better understanding of thevalues you need to specify in ANSYS CFX-Pre when creating a User CEL Function. Thecfx5mkext command is used to create the required objects and libraries as describedbelow. 3. From the main menu, select Tools > Command Editor. 4. Type the following in the Command Editor dialog box (make sure you do not miss thesemi-colon at the end of the line): ! system ("cfx5mkext PipeValve_inlet.F") < 1 or die; • This is equivalent to executing the following at an OS command prompt: cfx5mkext PipeValve_inlet.F • The ! indicates that the following line is to be interpreted as power syntax and not CCL. Everything after the ! symbol is processed as Perl commands. • system is a Perl function to execute a system command. • The < 1 or die will cause an error message to be returned if, for some reason, there is an error in processing the command. 5. Click Process to compile the subroutine.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 173Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.185. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreThe output produced when this command is executed will be printed to your terminalwindow.Note: You can use the -double option (that is, cfx5mkext -double PipeValve_inlet.F)to compile the subroutine for use with double precision.A subdirectory will have been created in your working directory whose name is systemdependent (for example, on IRIX it is named irix). This subdirectory contains theshared object library.Note: If you are running problems in parallel over multiple platforms then you will need tocreate these subdirectories using the cfx5mkext command for each different platform.•You can view more details about the cfx5mkext command by running cfx5mkext -help•You can set a Library Name and Library Path using the -name and -dest options respectively.•If these are not specified, the default Library Name is that of your Fortran file and the default Library Path is your current working directory.6. Close the Command Editor dialog box.Creating the Input ArgumentsNext, you will create some values that will be used as input arguments when the subroutineis called.1. Click Expression .2. Set Name to Wmax, and then click OK.3. Type 5 [m s^-1] into the Definition box, and then click Apply. The expression will be listed in the Expressions tree view.4. Use the same method to create an expression named Rmax defined to be 20 [mm].Creating the User CEL FunctionTwo steps are required to define a User CEL Function that uses the compiled Fortransubroutine. First, a User Routine that points to the Fortran subroutine will be created. Thena User CEL Function that points to the User Routine will be created.1. From the main toolbar, click User Routine.2. Set Name to WprofRoutine, and then click OK. The User Routine details view appears.3. Set Option to User CEL Function.4. Set Calling Name to inlet_velocity.•This is the name of the subroutine within the Fortran file.•Always use lower case letters for the calling name, even if the subroutine name in the Fortran file is in upper case.5. Set Library Name to PipeValve_inlet.•This is the name passed to the cfx5mkext command by the -name option.•If the -name option is not specified, a default is used.Page 174 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.186. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre •The default is the Fortran file name without the .F extension. 6. Set Library Path to the directory where the cfx5mkext command was executed(usually the current working directory). For example: •UNIX: /home/user/cfx/tutorials/PipeValve. •Windows: c:usercfxtutorialsPipeValve.This can be accomplished quickly by clicking Browse (next to Library Path),browsing to the appropriate folder in Select Directory (not necessary if selectingthe working directory), and clicking OK (in Select Directory). 7. Click OK to complete the definition of the user routine. 8. Click User Function. 9. Set Name to WprofFunction, and then click OK.The Function details view appears. Important: You must not use the same name for the function and the routine. 10. Set Option to User Function. 11. Set User Routine Name to WprofRoutine. 12. Set Argument Units to [m s^-1], [m], [m]. These are the units for the three input arguments: Wmax, r, and Rmax. Set Result Units to [m s^-1], since the result will be a velocity for the inlet. 1. Click OK to complete the User Function specification.You can now use the user function (WprofFunction) in place of a velocity value byentering the expression WprofFunction(Wmax, r, Rmax) (although it only makessense for the W component of the inlet velocity in this tutorial).In the definition of WprofFunction, the variable r (radius) is a system variable definedas: 22 r = x +y(Eqn. 3) In this equation, x and y are defined as directions 1 and 2 (X and Y for Cartesian coordinate frames) respectively, in the selected reference coordinate frame.Creating the Boundary ConditionsInlet Boundary 1. Create a new boundary condition named inlet. 2. Apply the following settings Tab Setting Value Basic SettingsBoundary Type Inlet LocationinletANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 175Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.187. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreTabSetting ValueBoundary Mass And Momentum > OptionCart. Vel. ComponentsDetailsMass And Momentum > U 0 [m s^-1] Mass And Momentum > V 0 [m s^-1] Mass And Momentum > W Wprof -OR- WprofFunction(Wmax, r, Rmax)*Fluid Values†Boundary Conditions Sand Fully Coupled Sand Fully Coupled > Particle Behavior > Define (Selected) Particle Behavior Sand Fully Coupled > Mass and Momentum >Cart. Vel. Components‡ Option Sand Fully Coupled > Mass And Momentum > U0 [m s^-1] Sand Fully Coupled > Mass And Momentum > V0 [m s^-1] Sand Fully Coupled > Mass And Momentum > WWprof -OR- WprofFunction(Wmax, r, Rmax)** Sand Fully Coupled > Particle Position > Option Uniform Injection Sand Fully Coupled > Particle Position > Number Direct Specification of Positions > Option Sand Fully Coupled > Particle Position > Number 200 of Positions > Number Sand Fully Coupled > Particle Mass Flow > Mass0.01 [kg s^-1] Flow RateFluid Values Boundary Conditions Sand One Way Coupled Sand One Way Coupled > Particle Behavior >(Selected) Define Particle Behavior Sand One Way Coupled > Mass and Momentum > Cart. Vel. Components†† Option Sand One Way Coupled > Mass And Momentum > 0 [m s^-1] U Sand One Way Coupled > Mass And Momentum > 0 [m s^-1] V Sand One Way Coupled > Mass And Momentum > Wprof -OR- WWprofFunction(Wmax,r, Rmax)‡‡ Sand One Way Coupled > Particle Position >Uniform Injection Option Sand One Way Coupled > Particle Position >Direct Specification Number of Positions > Option Sand One Way Coupled > Particle Position >5000 Number of Positions > Number Sand One Way Coupled > Particle Position >0.01 [kg s^-1] Particle Mass Flow Rate > Mass Flow RatePage 176 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.188. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-Pre *.Use the Expressions details view to enter either Wprof if using the expression method, or WprofFunction(Wmax, r, Rmax) if using the User CEL Function method. †. Do NOT select Particle Diameter Distribution. The diameter distribution was defined when creating the domain; this option would override those settings for this boundary only. ‡. Instead of manually specifying the same velocity profile as the fluid, you can also select the Zero Slip Velocity option. **. as you did on the Boundary Details tab ††. Instead of manually specifying the same velocity profile as the fluid, you can also select the Zero Slip Velocity option. ‡‡. as you did on the Boundary Details tab 3. Click OK. One-way coupled particles are tracked as a function of the fluid flow field. The latter is not influenced by the one-way coupled particles. The fluid flow will therefore be influenced by the 0.01 [kg s^-1] flow of two-way coupled particles, but not by the 0.01 [kg s^-1] flow of one-way coupled particles.Outlet 1. Create a new boundary condition named outlet.Boundary 2. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Outlet LocationoutletBoundary Flow Regime > OptionSubsonicDetailsMass and Momentum > OptionAverage Static Pressure Mass and Momentum > Relative Pressure 0 [Pa] 3. Click OK.Symmetry Plane 1. Create a new boundary condition named symP.Boundary 2. Apply the following settingsTabSetting ValueBasic Settings Boundary Type Symmetry LocationsymP 3. Click OK.Pipe Wall1. Create a new boundary condition named pipe wall.Boundary 2. Apply the following settingsTabSetting ValueBasicBoundary Type WallSettings Locationpipe wallANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 177Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.189. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreTabSetting ValueBoundary Wall Roughness > Option Rough WallDetailsRoughness Height0.2 [mm]*FluidBoundary Conditions Sand Fully CoupledValues Boundary Conditions > Sand Fully Coupled > Velocity Restitution Coefficient > Option Boundary Conditions > Sand Fully Coupled > Velocity 0.8 > Perpendicular Coeff. Boundary Conditions > Sand Fully Coupled > Velocity 1 > Parallel Coeff. Boundary Conditions Sand One Way Coupled Boundary Conditions > Sand One Way Coupled >Restitution Coefficient Velocity > Option Boundary Conditions > Sand One Way Coupled >0.8 Velocity > Perpendicular Coeff. Boundary Conditions > Sand One Way Coupled >1 Velocity > Parallel Coeff. *.Make sure that you change the units to millimetres. The thickness of the first element should be of the same order as the roughness height.3. Click OK.Editing the 1. In the Outline tree view, edit the boundary condition named Default DomainDefaultDefault.Boundary2. Apply the following settingsConditionTabSetting ValueFluid Values Boundary Conditions Sand Fully Coupled Boundary Conditions > Sand Fully0.9 Coupled > Velocity > Perpendicular Coeff. Boundary Conditions Sand One Way Coupled Boundary Conditions > Sand One Way0.9 Coupled > Velocity > Perpendicular Coeff.3. Click OK.Setting Initial Values1. Click Global Initialization .2. Apply the following settingsPage 178 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.190. Tutorial 9: Flow Through a Butterfly Valve: Defining a Simulation in ANSYS CFX-PreTab SettingValueGlobal Settings Initial Conditions > Cartesian VelocityAutomatic with ValueComponents > OptionInitial Conditions > Cartesian Velocity0 [m s^-1]Components > Option > UInitial Conditions > Cartesian Velocity0 [m s^-1]Components > Option > VInitial Conditions > Cartesian VelocityWprof -OR-Components > Option > WWprofFunction(Wmax, r, Rmax)*Initial Conditions > Turbulence Eddy (Selected)Dissipation *.Use Enter Expressionto enter Wprof if using the Expression method; enter WprofFunction(Wmax, r, Rmax) if using the User CEL Function method. 3. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settingsTabSettingValueBasic Settings Advection Scheme > OptionSpecified Blend Factor Advection Scheme > Blend Factor0.75Particle Control Particle Integration > Maximum Tracking Time (Selected) Particle Integration > Maximum Tracking Time 10 [s] > Value Particle Integration > Maximum Tracking(Selected) Distance Particle Integration > Maximum Tracking10 [m] Distance > Value Particle Integration > Max. Num. Integration (Selected) Steps Particle Integration > Max. Num. Integration 10000 Steps > Value Particle Integration > Max. Particle Intg. Time(Selected) Step Particle Integration > Max. Particle Intg. Time1e+10 [s] Step > Value 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 179Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.191. Tutorial 9: Flow Through a Butterfly Valve: Obtaining a Solution using ANSYS CFX-Solver ManagerWriting the Solver (.def) File1. Click Write Solver File .2. Apply the following settings:Setting ValueFile name PipeValve.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode.3. Ensure Start Solver Manager is selected and click Save.4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a Solution using ANSYS CFX-Solver ManagerWhen ANSYS CFX-Pre has shut down and ANSYS CFX-Solver Manager has started, you canobtain a solution to the CFD problem by using the following procedure.Note: If you followed the User CEL Function method, and you wish to run this tutorial indistributed parallel on machines with different architectures, you must first compile thePipeValve_inlet.F subroutine on all architectures.1. Ensure the Define Run dialog box is displayed and click Start Run.2. Click Yes to post-process the results when the completion message appears at the end of the run.3. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-PostIn this section, you will first plot erosion on the valve surface and side walls due to the sandparticles. You will then create an animation of particle tracks through the domain.Erosion Due to Sand ParticlesAn important consideration in this simulation is erosion to the pipe wall and valve due to thesand particles. A good indication of erosion is given by the Erosion Rate Densityparameter, which corresponds to pressure and shear stress due to the flow.1. Edit the object named Default Domain Default.2. Apply the following settings using the Ellipsisas required for selectionsPage 180 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.192. Tutorial 9: Flow Through a Butterfly Valve: Viewing the Results in ANSYS CFX-PostTabSetting ValueColorModeVariable VariableSand One Way Coupled.Erosion Rate Density* Range User Specified Min 0 [kg m^-2 s^-1] Max 25 [kg m^-2 s^-1]† *.This is statistically better than Sand Fully Coupled.Erosion Rate Density since many more particles were calculated for Sand One Way Coupled. †.This range is used to gain a better resolution of the wall shear stress values around the edge of the valve surfaces. 3. Click Apply. As can be seen, the highest values occur on the edges of the valve where most particles strike. Erosion of the low Z side of the valve would occur more quickly than for the high Z side.Particle Tracks Default particle track objects are created at the start of the session. One particle track is created for each set of particles in the simulation. You are going to make use of the default object for Sand Fully Coupled. The default object draws 10 tracks as lines from the inlet to outlet. Info shows information about the total number of tracks, index range and the track numbers which are drawn. 1. Edit the object named Res PT for Sand Fully Coupled. 2. Apply the following settingsTabSettingValueGeometry Max Tracks 20 3. Click Apply.Erosion on the Pipe Wall The User Specified range for coloring will be set to resolve areas of stress on the pipe wall near of the valve. 1. Clear the check box next to Res PT for Sand Fully Coupled. 2. Clear the check box next to Default Domain Default. 3. Edit the object named pipe wall. 4. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 181Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.193. Tutorial 9: Flow Through a Butterfly Valve: Viewing the Results in ANSYS CFX-PostTab Setting ValueColor ModeVariableVariableSand One Way Coupled.Erosion Rate DensityRange User SpecifiedMin 0 [kg m^-2 s^-1]Max 25 [kg m^-2 s^-1]5. Click Apply.Particle Track Symbols1. Clear visibility for all objects except Wireframe.2. Edit the object named Res PT for Sand Fully Coupled.3. Apply the following settingsTab Setting ValueColor ModeVariableVariableSand Fully Coupled.Velocity wSymbolDraw Symbols(Selected)Draw Symbols > Max Time 0 [s]Draw Symbols > Min Time 0 [s]Draw Symbols > Interval 0.07 [s]Draw Symbols > Symbol Fish3DDraw Symbols > Symbol Size0.54. Clear Draw Tracks.5. Click Apply.Symbols are placed at the start of each track.Creating a Particle Track AnimationThe following steps describe how to create a particle tracking animation using QuickAnimation. Similar effects can be achieved in more detail using the Keyframe Animationoption, which allows full control over all aspects on an animation.1. Select Tools > Animation or click Animation.2. Select Quick Animation.3. Select Res PT for Sand Fully Coupled:4. Click Options to display the Animation Options dialog box, then clear Override Symbol Settings to ensure the symbol type and size are kept at their specified settings for the animation playback. Click OK.Note: The arrow pointing downward in the bottom right corner of the Animation Windowwill reveal the Options button if it is not immediately visible.Page 182 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.194. Tutorial 9: Flow Through a Butterfly Valve: Viewing the Results in ANSYS CFX-Post 5. Select Loop. 6. Deselect Repeat foreverand ensure Repeat is set to 1. 7. Select Save MPEG. 8. Click Browseand enter tracks.mpg as the file name. 9. Click Play the animation. 10. If prompted to overwrite an existing movie, click Overwrite. The animation plays and builds an .mpg file. 11. Close the Animation dialog box.Performing Quantitative Calculations On the outlet boundary condition you created in ANSYS CFX-Pre, you set the Average Static Pressure to 0.0 [Pa]. To see the effect of this: 1. From the main menu select Tools > Function Calculator.The Function Calculator is displayed. It allows you to perform a wide range ofquantitative calculations on your results. Note: You should use Conservative variable values when performing calculations and Hybrid values for visualization purposes. Conservative values are set by default in ANSYS CFX-Post but you can manually change the setting for each variable in the Variables Workspace, or the settings for all variables by using the Function Calculator. 2. Set Function to maxVal. 3. Set Location to outlet. 4. Set Variable to Pressure. 5. Click Calculate.The result is the maximum value of pressure at the outlet. 6. Perform the calculation again using minVal to obtain the minimum pressure at theoutlet. 7. Select areaAve, and then click Calculate. • This calculates the area weighted average of pressure. • The average pressure is approximately zero, as specified by the boundary condition.Other Features The geometry was created using a symmetry plane. You can display the other half of the geometry by creating a YZ Plane at X = 0 and then editing the Default Transform object to use this plane as a reflection plane. 1. When you have finished viewing the results, quit ANSYS CFX-Post.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 183Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.195. Tutorial 9: Flow Through a Butterfly Valve: Viewing the Results in ANSYS CFX-PostPage 184 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.196. Tutorial 10:Flow in a Catalytic ConverterIntroduction This tutorial includes: • Tutorial 10 Features (p. 185) • Overview of the Problem to Solve (p. 186) • Defining a Simulation in ANSYS CFX-Pre (p. 187) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 193) • Viewing the Results in ANSYS CFX-Post (p. 194) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 187). Sample files referenced by this tutorial include: • CatConv.pre • CatConvHousing.hex • CatConvMesh.gtmTutorial 10 Features This tutorial addresses the following features of ANSYS CFX.ANSYS CFX TutorialsPage 185ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.197. Tutorial 10: Flow in a Catalytic Converter: Overview of the Problem to SolveComponent Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateFluid TypeIdeal GasTurbulence Modelk-EpsilonHeat Transfer IsothermalSubdomainsResistance SourceBoundary Conditions Inlet (Subsonic)Outlet (Subsonic)Wall: No-SlipDomain Interfaces Fluid-Fluid (No Frame Change)TimestepPhysical Time ScaleANSYS CFX-PostPlots ContourDefault LocatorsOutline Plot (Wireframe)PolylineSlice PlaneVectorOther Chart CreationData ExportTitle/TextViewing the Mesh In this tutorial you will learn about: • Using multiple meshes in ANSYS CFX-Pre. • Joining meshes together using static fluid-fluid domain interfaces between the inlet/outlet flanges and the central catalyst body. • Applying a source of resistance using a directional loss model. • Creating a chart to show pressure drop through the domain in ANSYS CFX-Post. • Exporting data from a line locator to a file.Overview of the Problem to Solve Catalytic converters are used on most vehicles on the road today. They reduce harmful emissions from internal combustion engines (such as oxides of nitrogen, hydrocarbons, and carbon monoxide) that are the result of incomplete combustion. Most new catalyticPage 186ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.198. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-Pre converters are the honeycomb ceramic type and are usually coated with platinum, rhodium, or palladium. The exhaust gases flow through the honeycomb structure and a pressure gradient is established between the inlet and outlet.exhaust gas25.0 m/s288.0 Kcatalyst material flange20 cm In this tutorial, a catalytic converter is modeled without chemical reactions in order to determine the pressure drop. The inlet flange (joining the pipe to the catalyst) is designed to distribute exhaust gas evenly across the catalyst material. A hexahedral mesh for the housing, which was created in ICEM-Hexa, is provided. The different meshes are connected together in ANSYS CFX-Pre. You will import each mesh then create a domain, which spans all of them. Within the converter, a subdomain is added to model a honeycomb structure using a directional loss model. The physics is then specified in the same way as for other tutorials.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: CatConv.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 193).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 187Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.199. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-Pre 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type CatConv. 6. Click Save.Importing the Meshes The catalytic converter is comprised of three distinct parts: • The inlet section (pipe and flange). • The outlet section (pipe and flange). • The catalyst (or monolith). Next you will import a generic inlet/outlet section and the catalyst housing from provided files.Housing Section The first mesh that you will import is the hexahedral mesh for the catalyst housing, createdin ICEM-Hexa, named CatConvHousing.hex. This mesh was created using units ofcentimetres; however, the units are not stored with the mesh file for this type of mesh. Youmust set the mesh import units to cm when importing the mesh into ANSYS CFX-Pre so thatthe mesh remains the intended size. The imported mesh has a width in the x-direction of 21cm and a length in the z-direction of 20 cm. 1. Right-click Mesh and select Import Mesh. 2. Apply the following settings Setting Value File type All Types Definition > Mesh FormatICEM CFD File name CatConvHousing.hex Definition > Mesh Units cm 3. Click Open.Pipe and FlangeThis mesh was created in units of centimetres. When importing GTM files, ANSYS CFX-PreSectionuses the units used in the mesh file. 1. Right-click Mesh and select Import Mesh to import the second section. 2. Apply the following settings Setting Value File type CFX Mesh (gtm) File name CatConvMesh.gtm 3. Click Open. You only need to import this mesh once, as you will be copying and rotating the flange through 180 degrees in the next step to create the inlet side pipe and flange.Page 188ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.200. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-PreApplying a Transform The pipe and flange are located at the outlet end of the housing. The flange will be rotated about an axis that points in the y-direction and is located at the center of the housing. 1. Right-click CatConvMesh.gtm and select Transform Mesh. The Mesh TransformationEditor dialog box appears. 2. Apply the following settingsTab Setting ValueDefinitionApply Rotation > Rotation OptionRotation AxisApply Rotation > From 0, 0, 0.16Apply Rotation > To 0, 1, 0.16*Apply Rotation > Rotation Angle 180 [degree]Multiple Copies (Selected)Multiple Copies > # of Copies 1 *.This specifies an axis located at the center of the housing parallel to the y-axis. 3. Click OK.Creating a Union Region Three separate regions now exist, but since there is no relative motion between each region, you only need to create a single domain. This can be done by simply using all three regions in the domain Location list or, as in this case, by using the Region details view to create a union of the three regions. 1. Create a new composite region named CatConverter. 2. Apply the following settingsTab SettingValueBasic SettingsDimension (Filter) 3DRegion ListB1.P3, B1.P3 2, LIVE 3. Click OK.Creating the Domain For this simulation you will use an isothermal heat transfer model and assume turbulent flow. 1. Click Domainand set the name to CatConv. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 189Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.201. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-PreTabSetting ValueGeneralBasic Settings > Location CatConverterOptions Basic Settings > Fluid List Air Ideal Gas Domain Models > Pressure > Reference Pressure 1 [atm]Fluid Models Heat Transfer > OptionIsothermal Heat Transfer > Fluid Temperature 600 [K]3. Click OK.Creating a Subdomain to Model the Catalyst StructureThe catalyst-coated honeycomb structure will be modeled using a subdomain with adirectional source of resistance.For quadratic resistances, the pressure drop is modeled using:∂p ------ = – K Q U U i- (Eqn. 1) ∂x iwhere K Q is the quadratic resistance coefficient, U i is the local velocity in the i direction,∂pand ------ is the pressure drop gradient in the i direction. -∂x i1. Select Insert > Subdomain from the main menu or click Subdomain2. In the Insert Subdomain dialog box, type catalyst.3. Apply the following settingsTabSetting ValueBasic Settings LocationLIVE*Sources† Sources (Selected) Sources > Momentum Source/Porous Loss (Selected) Sources > Momentum Source/Porous Loss > (Selected) Directional Loss *. This is the entire housing section. †. Used to set sources of momentum, resistance and mass for the subdomain (Othersources are available for different problem physics).4. Apply the following settings in the Directional Loss sectionSetting ValueStreamwise Direction > X Component0Streamwise Direction > Y Component0Streamwise Direction > Z Component1Page 190 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.202. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-PreSetting ValueStreamwise Loss > OptionLinear and QuadraticCoefsStreamwise Loss > Quadratic Resistance Coefficient(Selected)Streamwise Loss > Quadratic Resistance Coefficient > Quadratic650 [kg m^-4]Coefficient 5. Click OK.Creating Boundary ConditionsInlet Boundary 1. Create a new boundary condition named Inlet. 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type InletLocationPipeEnd 2Boundary DetailsMass and Momentum > Normal Speed25 [m s^-1] 3. Click OK.Outlet 1. Create a new boundary condition named Outlet.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type OutletLocationPipeEndBoundary DetailsMass and Momentum > OptionStatic PressureMass and Momentum > Relative Pressure 0 [Pa] 3. Click OK. The remaining surfaces are automatically grouped into the default no slip wall boundary condition.Creating the Domain Interfaces Domain interfaces are used to define the connecting boundaries between meshes where the faces do not match or when a frame change occurs. Meshes are ‘glued’ together using the General Grid Interface (GGI) functionality of ANSYS CFX. Different types of GGI connections can be made. In this case, you require a simple Fluid-Fluid Static connection (no Frame Change). Other options allow you to change reference frame across the interface or create a periodic boundary with dissimilar meshes on each periodic face. Two Interfaces are required, one to connect the inlet flange to the catalyst housing and one to connect the outlet flange to the catalyst housing.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 191Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.203. Tutorial 10: Flow in a Catalytic Converter: Defining a Simulation in ANSYS CFX-PreInlet Pipe /1. Create a new domain interface named InletSide.Housing 2. Apply the following settingsInterfaceTabSetting ValueBasic Settings Interface Side 1 > Region ListFlangeEnd 2 Interface Side 2 > Region ListINLET3. Click OK.Outlet Pipe / 1. Create a new domain interface named OutletSide.Housing 2. Apply the following settingsInterfaceTabSetting ValueBasic Settings Interface Side 1 > Region ListFlangeEnd Interface Side 2 > Region ListOUTLET3. Click OK.Setting Initial ValuesA sensible guess for the initial velocity is to set it to the expected velocity through thecatalyst housing. As the inlet velocity is 25 [m s^-1] and the cross sectional area of the inletand housing are known, you can apply conservation of mass to obtain an approximatevelocity of 2 [m s^-1] through the housing.1. Click Global Initialization .2. Apply the following settingsTabSetting ValueGlobal Initial Conditions > Cartesian Velocity Automatic with ValueSettings Components > Option Initial Conditions > Cartesian Velocity 0 [m s^-1] Components > U Initial Conditions > Cartesian Velocity 0 [m s^-1] Components > V Initial Conditions > Cartesian Velocity -2 [m s^-1] Components > W Initial Conditions > Turbulence Eddy(Selected) Dissipation3. Click OK.Setting Solver ControlAssuming velocities of 25 [m s^-1] in the inlet and outlet pipes, and 2 [m s^-1] in the catalysthousing, an approximate fluid residence time of 0.1 [s] can be calculated. A sensibletimestep of 0.04 [s] (1/4 to 1/2 of the fluid residence time) will be applied.Page 192 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.204. Tutorial 10: Flow in a Catalytic Converter: Obtaining a Solution using ANSYS CFX-Solver Manager For the convergence criteria, an RMS value of at least 1e-05 is usually required for adequate convergence, but the default value is sufficient for demonstration purposes. 1. Click Solver Control . 2. Apply the following settingsTab Setting ValueBasic SettingsConvergence Control > Fluid Timescale Physical TimescaleControl > Timescale ControlConvergence Control >Fluid Timescale0.04 [s]Control > Physical Timescale 3. Click OK.Writing the Solver (.def) File While writing the solver file, you will use the Summarize Interface Data option to display information about the connection type used for each domain interface. 1. Click Write Solver File. 2. Apply the following settingsSetting ValueFile name CatConv.defSummarize Interface Data(Selected)Quit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. Once ANSYS CFX-Solver Manager launches, return to ANSYS CFX-Pre.The Interface Summary dialog box is displayed. This displays information related to thesummary of interface connections. 5. Click OK. 6. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, you can obtain a solution to the CFD problem by following the instructions below: 1. Ensure Define Run is displayed. 2. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 193Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.205. Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-Post3. Click Yes to post-process the results.4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-PostWhen ANSYS CFX-Post opens, you will need to experiment with the Edge Angle setting forthe Wireframe object in order to view an appropriate amount of the mesh.Under the Outline tab, several interface boundaries are available. The two connectionsbetween the catalyst housing mesh and the mesh for the inlet and outlet pipes have twointerface boundaries each, one for each side of the connection.1. Zoom in so the geometry fills the viewer.2. In the Outline tree view, edit InletSide Side 1.3. Apply the following settingsTab SettingValueRenderDraw Faces (Cleared)Draw Lines (Selected)Draw Lines > Color ModeUser SpecifiedDraw Lines > Line Color(Red)4. Click Apply.5. In the Outline tree view, edit InletSide Side 2.6. Apply the following settingsTab SettingValueRenderDraw Faces (Cleared)Draw Lines (Selected)Draw Lines > Color ModeUser SpecifiedDraw Lines > Line Color(Green)7. Click Apply.8. In the Outline tree view, clear Wireframe to hide it.9. Right-click a blank area in the viewer and select Predefined Camera > View Towards -Z.You should now have a clear view of the tetrahedral / prism and hexahedral mesh on eachside of the interface. The General Grid Interface (GGI) capability of ANSYS CFX was used toproduce a connection between these two dissimilar meshes before the solution wascalculated. Notice that there are more tetrahedral / prism elements than hexahedralelements and that the extent of the two meshes is not quite the same (this is mostnoticeable on the curved edges). The extent of each side of the interface does not have tomatch to allow a GGI connection to be made.Page 194 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.206. Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-PostCreating User Locations and Plots 1. In the Outline tree view, select Wireframe to show it. 2. In the Outline tree view, clear both InletSide Side 1 and InletSide Side 2.Creating a Slice Plane 1. Create a new plane named Plane 1. 2. Apply the following settingsTab Setting ValueGeometryDefinition > Method ZX PlaneColor ModeVariableVariablePressure 3. Click Apply. 4. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Y.Creating a Contour Plot The pressure falls steadily throughout the main body of the catalytic converter. You can confirm this with a contour plot. 1. Clear Plane 1 in the Outline tab. 2. Create a new contour plot named Contour 1. 3. Apply the following settingsTab Setting ValueGeometryLocations Plane 1VariablePressure# of Contours 30RenderDraw Faces(Cleared) 4. Click Apply.Creating a Vector Plot Using the Slice Plane 1. Create a new vector plot named Vector 1. 2. Apply the following settingsTab Setting ValueGeometryLocations Plane 1SymbolSymbol Size 0.1Normalize Symbols (Selected) 3. Click Apply.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 195Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.207. Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-PostNotice the flow separates from the walls, where the inlet pipe expands into the flange,setting up a recirculation zone. The flow is uniform through the catalyst housing.Suppose for now that you want to see if the pressure drop is linear by plotting a line graphof pressure against the z-coordinate. In this case you will use ANSYS CFX-Post to produce thegraph, but you could also export the data, then read it into any standard plotting package.Graphs are produced using the chart object, but before you can create the chart you mustdefine the points at which you require the data. To define a set of points in a line, you canuse the polyline object.Creating a PolylineThe Method used to create the polyline can be From File, Boundary Intersection orFrom Contour. If you select From File, you must specify a file containing point definitionsin the required format.In this tutorial, you will use the Boundary Intersection method. This creates a polylinefrom the intersecting line between a boundary object and a location (e.g., between a walland a plane). The points on the polyline are where the intersecting line cuts through asurface mesh edge.You will be able to see the polyline following the intersecting line between the wall, inletand outlet boundaries and the slice plane.1. In the Outline tree view, clear Contour 1 and Vector 1.2. Create a new polyline named Polyline 1.3. Apply the following settingsTab Setting ValueGeometryMethodBoundary IntersectionBoundary List CatConv Default, Inlet, Outlet*Intersect WithPlane 1Color Color (Yellow)RenderLine Width3 *.Click the ellipsis icon to select multiple items using the key.4. Click Apply.5. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Y up).Creating a ChartNow that a polyline has been defined, a chart can be created. Charts are defined by creatingchart line objects. A chart line is listed in the tree view beneath the chart object to which itbelongs.1. Create a new chart named Chart 1.2. Apply the following settingsPage 196 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.208. Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-PostTab Setting ValueChart Title Pressure Drop through a CatalyticConverterChart Line 1Line Name Pressure DropLocationPolyline 1X Axis > Variable ZY Axis > Variable PressureAppearance > SymbolsRectangleAppearanceSizes > Line3 3. Click Apply.Through the main body of the catalytic converter you can see that the pressure drop islinear. This is in the region from approximately Z=0.05 to Z=0.25. The two lines show thepressure on each side of the wall. You can see a noticeable difference in pressurebetween the two walls on the inlet side of the housing (at around Z=0.25). 4. If required, in the Outline tree view, select Contour 1, Polyline 1, and Vector 1. 5. Click the 3D Viewer tab, then right-click a blank area and select Predefined Camera >View Towards +Y.You should now see that the flow enters the housing from the inlet pipe at a slight angle,producing a higher pressure on the high X wall of the housing. 6. Under Report, expand Chart 1, and edit Chart Line 1. 7. Apply the following settingsTab Setting ValueChart Line 1X Axis > Variable Chart Count* *.This is the data point number (e.g. 1,2,3,4...), it does NOT represent the distance between each point along the polyline. 8. Click Apply.Exporting Data 1. From the main menu, select File > Export. 2. Apply the following settingsTab Setting ValueOptions Locations Polyline 1Export Geometry Information (Selected)*Select VariablesPressureFormattingPrecision 3 *.This ensures X, Y, and Z to be sent to the output file. 3. Click Save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 197Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.209. Tutorial 10: Flow in a Catalytic Converter: Viewing the Results in ANSYS CFX-PostThe file export.csv will be written to the current working directory. This file can beopened in any text editor. You can use the exported data file to plot charts in othersoftware.4. When finished, quit ANSYS CFX-Post.Page 198 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.210. Tutorial 11:Non-Newtonian Fluid Flow inan AnnulusIntroduction This tutorial includes: • Tutorial 11 Features (p. 200) • Overview of the Problem to Solve (p. 201) • Defining a Simulation in ANSYS CFX-Pre (p. 201) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 205) • Viewing the Results in ANSYS CFX-Post (p. 206) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 201). Sample files referenced by this tutorial include: • NonNewton.pre • NonNewtonMesh.gtmANSYS CFX TutorialsPage 199ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.211. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Tutorial 11 FeaturesTutorial 11 FeaturesThis tutorial addresses the following features of ANSYS CFX. Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeGeneral Fluid Domain Type Single Domain Turbulence ModelLaminar Heat Transfer None Boundary Conditions Symmetry Plane Wall: No-Slip Wall: Moving CEL (CFX Expression Language) TimestepAuto Time Scale ANSYS CFX-PostPlots Sampling Plane Slice Plane VectorIn this tutorial you will learn about:• Using CFX Expression Language (CEL) to define the properties of a shear-thickeningfluid.• Using the Moving Wall feature to apply a rotation to the fluid at a wall boundary.Page 200 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.212. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Overview of the Problem to SolveOverview of the Problem to Solve In this example a non-Newtonian, shear-thickening liquid rotates in a 2D eccentric annular pipe gap. The motion, shown by the arrow, is brought about solely by viscous fluid interactions caused by the rotation of the inner pipe.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: NonNewton.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 205).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type NonNewton. 6. Click Save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 201Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.213. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Defining a Simulation in ANSYS CFX-PreImporting the Mesh1. Right-click Mesh and select Import Mesh.2. Apply the following settingsSetting ValueFile name NonNewtonMesh.gtm3. Click Open.Creating an Expression for Shear Rate Dependent ViscosityYou can use an expression to define the dependency of fluid properties on other variables.In this case, the fluid does not obey the simple linear Newtonian relationship between shearstress and shear strain rate. The general relationship for the fluid you will model is given by: n–1 µ = Kγ (Eqn. 1)where γ is the shear strain rate and K and n are constants. For your fluid, n =1.5 and thisresults in shear-thickening behavior of the fluid, i.e., the viscosity increases with increasingshear strain rate. The shear strain rate is available as a ANSYS CFX-Pre System Variable(sstrnr).In order to describe this relationship using CEL, the dimensions must be consistent on bothsides of the equation. Clearly this means that K must have dimensions and requires units tosatisfy the equation. If the units of viscosity are kg m^-1 s^-1, and those of γ are s^-1, thenthe expression is consistent if the units of K are kg m^-1 s^(-0.5).1. Create the following expressions, remembering to click Apply after each is defined.NameDefinitionK 10.0 [kg m^-1 s^-0.5]n 1.5You should bound the viscosity to ensure that it remains physically meaningful. To doso, you will create two additional parameters that will be used to guarantee the value ofthe shear strain rate.2. Create the following expressions for upper and lower bounds.NameDefinitionUpperS100 [s^-1]LowerS1.0E-3 [s^-1]ViscEqn K*(min(UpperS,max(sstrnr,LowerS))^(n-1))3. Close the Expressions tab.Page 202 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.214. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Defining a Simulation in ANSYS CFX-PreCreating a New Fluid 1. Create a new material named myfluid. 2. Apply the following settingsTabSettingValueBasic Settings Thermodynamic State(Selected)Material PropertiesEquation of State > Molar Mass 1 [kg kmol^-1]* Equation of State > Density1.0E+4 [kg m^-3] Specific Heat Capacity (Selected) Specific Heat Capacity > Specific Heat Capacity0 [J kg^-1 K^-1]† Reference State(Selected) Reference State > Option Specified Point Reference State > Ref. Temperature 25 [C] Reference State > Reference Pressure 1 [atm] Transport Properties > Dynamic Viscosity (Selected) Transport Properties > Dynamic Viscosity > ViscEqn Dynamic Viscosity *.This is not the correct Molar Mass value, but this material property will not be used by the ANSYS CFX-Solver for this case. In other cases it will be used. †.This is not the correct value for specific heat, but this property will not be used in the ANSYS CFX-Solver. 3. Click OK.Creating the Domain 1. Click Domainand set the name to NonNewton. 2. Apply the following settings to NonNewtonTab Setting ValueGeneral Basic Settings > Fluids ListmyfluidOptions Domain Models > Pressure > Reference Pressure 1 [atm]Fluid ModelsHeat Transfer > OptionIsothermalHeat Transfer > Fluid Temperature 25 CTurbulence > Option None (Laminar) 3. Click OK.Creating the Boundary ConditionsWall Boundary1. Create a new boundary condition named rotwall. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 203Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.215. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic SettingsBoundary TypeWallLocation rotwallBoundary DetailsWall Influence on Flow > Wall Velocity (Selected)Wall Influence on Flow > Wall Velocity > Rotating WallOptionWall Influence on Flow > Wall Velocity > 31.33 [rev min^-1]Angular Velocity3. Click OK.Symmetry Plane 1. Create a new boundary condition named SymP1.Boundary 2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeSymmetryLocation SymP13. Click OK.4. Create a new boundary condition named SymP2.5. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeSymmetryLocation SymP26. Click OK.The outer annulus surfaces will default to the no-slip stationary wall boundarycondition.Setting Initial ValuesA reasonable initial guess for the velocity field is a value of zero throughout the domain.1. Click Global Initialization .2. Apply the following settingsTabSetting ValueGlobal Initial Conditions > Cartesian Velocity Components > Option Automatic withSettings Value Initial Conditions > Cartesian Velocity Components > U0 [m s^-1] Initial Conditions > Cartesian Velocity Components > V0 [m s^-1] Initial Conditions > Cartesian Velocity Components > W0 [m s^-1]3. Click OK.Page 204 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.216. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Obtaining a Solution using ANSYS CFX-Solver ManagerSetting Solver Control 1. Click Solver Control. 2. Apply the following settingsTab SettingValueBasic SettingsAdvection Scheme > OptionSpecific Blend FactorAdvection Scheme > Blend Factor1*Convergence Control > Max. Iterations50Convergence Criteria > Residual Target 1e-05 *.This is the most accurate but least robust advection scheme. 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File . 2. Apply the following settings:Setting ValueFile name NonNewton.defQuit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, you can obtain a solution to the CFD problem by following the instructions below: 1. Ensure Define Run is displayed. 2. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed. 3. Click Yes to post-process the results. 4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 205Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.217. Tutorial 11: Non-Newtonian Fluid Flow in an Annulus: Viewing the Results in ANSYS CFX-PostViewing the Results in ANSYS CFX-PostIn this tutorial you have used CEL to create an expression for the dynamic viscosity. If younow perform calculations or color graphics objects using the Dynamic Viscosity variable, itsvalues will have been calculated from the expression you defined in ANSYS CFX-Pre.These steps instruct the user on how to create a vector plot to show the velocity values inthe domain.1. Right-click a blank area in the viewer and select Predefined Camera > View Towards -Z from the shortcut menu.2. Create a new plane named Plane 1.3. Apply the following settingsTab SettingValueGeometryDefinition > MethodPoint and NormalDefinition > Point 0, 0, 0.02Definition > Normal0, 0, 1Plane Bounds > TypeCircularPlane Bounds > Radius0.3 [m]Plane Type SamplePlane Type > R Samples 32Plane Type > Theta Samples 24RenderDraw Faces (Cleared)4. Click Apply.5. Create a new vector plot named Vector 1.6. Apply the following settingsTab SettingValueGeometryDefinition > Locations Plane 1Definition > VariableVelocitySymbolSymbol Size37. Click Apply.8. Try creating some plots of your own, including one that shows the variation of dynamic viscosity.9. When you have finished, quit ANSYS CFX-Post.Page 206 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.218. Tutorial 12:Flow in an Axial Rotor/StatorIntroduction This tutorial includes: • Tutorial 12 Features (p. 208) • Overview of the Problem to Solve (p. 209) • Defining a Frozen Rotor Simulation in ANSYS CFX-Pre (p. 210) • Obtaining a Solution to the Frozen Rotor Model (p. 214) • Viewing the Frozen Rotor Results in ANSYS CFX-Post (p. 215) • Setting up a Transient Rotor-Stator Calculation (p. 216) • Obtaining a Solution to the Transient Rotor-Stator Model (p. 219) • Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post (p. 220) If this is the first tutorial you are working with it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 211). Sample files referenced by this tutorial include: • Axial.pre • AxialIni.pre • AxialIni_001.res • rotor.grd • stator.gtmANSYS CFX TutorialsPage 207ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.219. Tutorial 12: Flow in an Axial Rotor/Stator: Tutorial 12 FeaturesTutorial 12 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode Turbo WizardSimulation Type Steady StateTransientFluid TypeIdeal GasDomain Type Multiple DomainRotating Frame of ReferenceTurbulence Modelk-EpsilonHeat Transfer Total EnergyBoundary Conditions Inlet (Subsonic)Outlet (Subsonic)Wall: No-SlipWall: AdiabaticDomain Interfaces Frozen RotorPeriodicTransient Rotor StatorTimestepPhysical Time ScaleTransient ExampleTransient Results FileANSYS CFX-Solver ManagerRestartParallel ProcessingANSYS CFX-PostPlots AnimationIsosurfaceSurface GroupTurbo PostOther Changing the Color RangeChart CreationInstancing TransformationMPEG GenerationQuantitative CalculationTime Step SelectionTransient Animation In this tutorial you will learn about: • Using the Turbo Wizard in ANSYS CFX-Pre to quickly specify a turbomachinery application. • Multiple Frames of Reference and Generalized Grid Interface. • Using a Frozen Rotor interface between the rotor and stator domains. • Modifying an existing simulation. • Setting up a transient calculation. • Using a Transient Rotor-Stator interface condition to replace a Frozen Rotor interface.Page 208ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.220. Tutorial 12: Flow in an Axial Rotor/Stator: Overview of the Problem to Solve • Creating a transient animation showing domain movement in ANSYS CFX-Post.Overview of the Problem to Solve The following tutorial demonstrates the versatility of GGI and MFR in ANSYS CFX-Pre by combining two dissimilar meshes. The first mesh to be imported (the rotor) was created in CFX-TASCflow. This is combined with a second mesh (the stator) which was created using ANSYS CFX-Mesh. The geometry to be modeled consists of a single stator blade passage and two rotor blade passages. The rotor rotates about the Z-axis while the stator is stationary. Periodic boundaries are used to allow only a small section of the full geometry to be modeled. Figure 1 Geometry subsectionOutflow Shroud Stator BladeRotor BladeHub Inflow At the change in reference frame between the rotor and stator, two different interface models are considered. First a solution is obtained using a Frozen Rotor model. After viewing the results from this simulation, the latter is modified to use a transient rotor-stator interface model. The Frozen Rotor solution is used as an initial guess for the transient rotor-stator simulation.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 209Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.221. Tutorial 12: Flow in an Axial Rotor/Stator: Defining a Frozen Rotor Simulation in ANSYS CFX-PreThe full geometry contains 60 stator blades and 113 rotor blades. To help you visualize howthe modeled geometry fits into the full geometry, the following figure shows approximatelyhalf of the full geometry. The Inflow and Outflow labels show the location of the modeledsection in . Outflow InflowAxis of RotationAs previously indicated, the modeled geometry contains two rotor blades and one statorblade. This is an approximation to the full geometry since the ratio of rotor blades to statorblades is close to, but not exactly, 2:1. In the stator blade passage a 6° section is beingmodeled (360°/60 blades), while in the rotor blade passage a 6.372° section is beingmodeled (2*360°/113 blades). This produces a pitch ratio at the interface between the statorand rotor of 0.942. As the flow crosses the interface it is scaled to allow this type of geometryto be modeled. This results in an approximation of the inflow to the rotor passage.Furthermore, the flow across the interface will not appear continuous due to the scalingapplied.The periodic boundary conditions will introduce an additional approximation since theycannot be periodic when a pitch change occurs.You should always try to obtain a pitch ratio as close to 1 as possible in your model tominimize approximations, but this must be weighed against computational resources. A fullmachine analysis can be performed (modeling all rotor and stator blades) which will alwayseliminate any pitch change, but will require significant computational time. For thisrotor/stator geometry, a 1/4 machine section (28 rotor blades, 15 stator blades) wouldproduce a pitch change of 1.009, but this would require a model about 15 times larger thanin this tutorial example.Defining a Frozen Rotor Simulation in ANSYS CFX-PreThe following sections describe the simulation setup in ANSYS CFX-Pre.Page 210 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.222. Tutorial 12: Flow in an Axial Rotor/Stator: Defining a Frozen Rotor Simulation in ANSYS CFX-PrePlaying a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: AxialIni.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution to the Frozen Rotor Model (p. 214).Creating a New Simulation This tutorial will use the Turbomachinery wizard in ANSYS CFX-Pre. This pre-processing mode is designed to simplify the setup of turbomachinery simulations. 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select Turbomachinery and click OK. 4. Select File > Save Simulation As. 5. Under File name, type AxialIni. 6. Click Save.Basic Settings 1. Set Machine Type to Axial Turbine. 2. Click Next.Component Definition Two new components are required. As they are created, meshes are imported. 1. Right-click in the blank area and select New Component from the shortcut menu. 2. Create a new component of type Stationary, named S1. 3. Apply the following settingSetting ValueMesh > File stator.gtm* *.You may have to select the CFX Mesh option under File Type. 4. Create a new component of type Rotating, named R1. 5. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 211Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.223. Tutorial 12: Flow in an Axial Rotor/Stator: Defining a Frozen Rotor Simulation in ANSYS CFX-PreSettingValueComponent Type > Value 523.6 [radian s^-1]Mesh File > File rotor.grd* *.You may have to select the CFX-TASCflow option under File Type.Note: The components must be ordered as above (stator then rotor) in order for theinterface to be created correctly. The order of the two components can be changed by rightclicking on S1 and selecting Move Component Up.When a component is defined, Turbo Mode will automatically select a list of regions thatcorrespond to certain boundary condition types. This information should be reviewedin the Region Information section to ensure that all is correct. This information will beused to help set up boundary conditions and interfaces. The upper case turbo regionsthat are selected (e.g., HUB) correspond to the region names in the CFX-TASCflow grdfile. CFX-TASCflow turbomachinery meshes use these names consistently.6. Click Next.Physics DefinitionIn this section, you will set properties of the fluid domain and some solver parameters.1. Apply the following settingsTabSetting ValuePhysicsFluid Air Ideal GasDefinition Simulation Type > TypeSteady State Model Data > Reference Pressure 0.25 [atm] Model Data > Heat TransferTotal Energy Model Data > Turbulence k-Epsilon Boundary Templates > P-Total Inlet Mass Flow Outlet (Selected) Boundary Templates > P-Total0 [atm] Boundary Templates > T-Total340 [K] Boundary Templates > Mass Flow Rate 0.06 [kg s^-1] Interface > Default TypeFrozen Rotor Solver Parameters > Convergence Control Physical Timescale Solver Parameters > Physical Timescale0.002 [s]* *.This time scale is approximately equal to 1 / ω , which is often appropriate for rotating machinery applications.2. Click Next.Page 212 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.224. Tutorial 12: Flow in an Axial Rotor/Stator: Defining a Frozen Rotor Simulation in ANSYS CFX-PreInterface Definition ANSYS CFX-Pre will try to create appropriate interfaces using the region names presented previously in the Region Information section. In this case, you should see that a periodic interface has been generated for both the rotor and the stator. These are required when modeling a small section of the true geometry. An interface is also required to connect the two components together across the frame change. 1. Review the various interfaces but do not change them. 2. Click Next.Boundary Definition ANSYS CFX-Pre will try to create appropriate boundary conditions using the region names presented previously in the Region Information section. In this case, you should see a list of boundary conditions that have been generated. They can be edited or deleted in the same way as the interface connections that were set up earlier. 1. Review the various boundary definitions but do not change them. 2. Click Next.Final Operations 1. Set Operation to Enter General Mode. 2. Click Finish.Writing the Solver (.def) File 1. Click Write Solver File . 2. Apply the following settings:Setting ValueFile name AxialIni.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion. You should see ANSYS CFX-Solver Manager appear.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 213Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.225. Tutorial 12: Flow in an Axial Rotor/Stator: Obtaining a Solution to the Frozen Rotor ModelObtaining a Solution to the Frozen Rotor Model Compared to previous tutorials, the mesh for this tutorial contains many more nodes (although it is still too coarse to perform a high quality CFD simulation). This results in a corresponding increase in solution time for the problem. Solving this problem in parallel is recommended, if possible. Your machine should have a minimum of 256MB of memory to run this tutorial. More detailed information about setting up ANSYS CFX to run in parallel is available. For details, see Tutorial 5: Flow Around a Blunt Body (p. 109). You can solve this example using Serial, Local Parallel or Distributed Parallel. • Obtaining a Solution in Serial (p. 214) • Obtaining a Solution With Local Parallel (p. 214) • Obtaining a Solution with Distributed Parallel (p. 215)Obtaining a Solution in Serial If you do not have a license to run ANSYS CFX in parallel you can run in serial by clicking the Start Run button when ANSYS CFX-Solver Manager has opened up. Solution time in serial is approximately 45 minutes on a 1GHz processor. 1. Click Start Run on the Define Run dialog box.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed. 2. Click Yes to start ANSYS CFX-Post. 3. If using Standalone Mode, quit ANSYS CFX-Solver Manager. When you are finished, proceed to Viewing the Frozen Rotor Results in ANSYS CFX-Post (p. 215).Obtaining a Solution With Local Parallel To run in local parallel, the machine you are on must have more than one processor. 1. Set Run Mode to PVM Local Parallel in the Define Run dialog box.This is the recommended method for most applications. 2. If required, click Add Partitionto add more partitions. By default, 2 partitions are assigned. 3. Click Start Run. 4. Click Yes to post-process the results when the completion message appears at the endof the run. 5. If using Standalone Mode, quit ANSYS CFX-Solver Manager. When you are finished, proceed to Viewing the Frozen Rotor Results in ANSYS CFX-Post (p. 215).Page 214ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.226. Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Frozen Rotor Results in ANSYS CFX-PostObtaining a Solution with Distributed Parallel 1. Set Run Mode to PVM Distributed Parallel in the Define Run dialog box.One partition should already be assigned to the host that you are logged into. 2. Click Insert Hostto specify a new parallel host. 3. In Select Parallel Hosts, select another host name (this should be a machine that youcan log into using the same user name). 4. Click Add, and then Close.The names of the two selected machines should be listed in the Host Name column ofthe Define Run dialog box. 5. Click Start Run. 6. Click Yes to post-process the results when the completion message appears at the endof the run. 7. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Frozen Rotor Results in ANSYS CFX-Post The Turbo-Post feature will be demonstrated in the following sections. This feature is designed to greatly reduce the effort taken to post-process turbomachinery simulations.Initializing Turbo-Post To initialize Turbo-Post, the properties of each component must be entered. This includes entering information about the inlet, outlet, hub, shroud, blade and periodic regions. 1. Click the Turbo tab.The Turbo Initialization dialog box is displayed, and asks you whether you want toauto-initialize all components. Note: If you do not see the Turbo Initialization dialog box, or as an alternative to using that dialog box, you can initialize all components by clicking the Initialize All Components button which is visible initially by default, or after double-clicking the Initialization object in the Turbo tree view. 2. Click Yes. The Turbo tree view shows the two components in domains R1 and S1. In this case, the initialization works without problems. If there was a problem initializing a component, this would be indicated in the tree view.Viewing Three Domain Passages Next, you will create an instancing transformation to plot three blade passages for the stator and six blade passages for the rotor. The instancing properties of each domain have already been entered during Initialization. In the next steps, you will create a surface group plot to color the blade and hub surfaces with the same variable.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 215Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.227. Tutorial 12: Flow in an Axial Rotor/Stator: Setting up a Transient Rotor-Stator Calculation 1. From the main menu, select Insert > Location > Surface Group. 2. Click OK.The default name is accepted. 3. Apply the following settings TabSettingValue Geometry LocationsR1 Blade, R1 Hub, S1 Blade, S1 Hub ColorMode VariableVariable Pressure 4. Click Apply. 5. Click the Turbo tab. 6. Open Plots > 3D View for editing. 7. Apply the following settings TabSettingValue 3D ViewInstancing > DomainR1Instancing > # of Copies 3 8. Click Apply. 9. Apply the following settings TabSettingValue 3D ViewInstancing > DomainS1Instancing > # of Copies 3 10. Click Apply.Blade Loading Turbo Chart In this section, you will create a plot of pressure around the stator blade at a given spanwise location. 1. In the Turbo tree view, double-click Blade Loading.This profile of the pressure curve is typical for turbomachinery applications. When you are finished viewing the chart, quit ANSYS CFX-Post.Setting up a Transient Rotor-Stator Calculation This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre. The existing frozen-rotor simulation is modified to define the transient rotor-stator simulation. If you have not already completed the frozen-rotor simulation, please refer to Defining a Frozen Rotor Simulation in ANSYS CFX-Pre (p. 210) before proceeding with the transient rotor-stator simulation.Page 216ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.228. Tutorial 12: Flow in an Axial Rotor/Stator: Setting up a Transient Rotor-Stator CalculationPlaying a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: Axial.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution to the Transient Rotor-Stator Model (p. 219). Note: The session file creates a new simulation named Axial.cfx and will not modify the existing database. It also copies the required initial values files from the examples directory to the current working directory.Opening the Existing Simulation This step involves opening the original simulation and saving it to a different location. 1. Start ANSYS CFX-Pre. 2. Open the results file named AxialIni_001.res. 3. Save the simulation as Axial.cfx in your working directory. 4. Select Tools > Turbo Mode. Basic Settings is displayedModifying the Physics Definition You need to modify the domain to define a transient simulation. You are going to run for a time interval such that the rotor blades pass through 1 pitch (6.372°) using 10 timesteps. This is generally too few timesteps to obtain high quality results, but is sufficient for tutorial purposes. The timestep size is calculated as follows: Rotational Speed = 523.6 rad/s Rotor Pitch Modelled = 2*(2π/113) = 0.1112 rad Time to pass through 1 pitch = 0.1112/523.6 = 2.124e-4 s Since 10 time steps are used over this interval each timestep should be 2.124e-5 s. 1. Click Next.Component Definition is displayed. 2. Click Next.Physics Definition is displayed. 3. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 217Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.229. Tutorial 12: Flow in an Axial Rotor/Stator: Setting up a Transient Rotor-Stator Calculation TabSettingValue PhysicsFluidAir Ideal Gas DefinitionSimulation Type > Type TransientSimulation Type > Total Time 2.124e-4 [s]*Simulation Type > Time Steps 2.124e-5 [s]†Interface > Default Type Transient Rotor Stator*.This gives 10 timesteps of 2.124e-5 s†.This timestep will be used until the total time is reached Note: A transient rotor-stator calculation often runs through more than one pitch. In these cases, it may be useful to look at variable data averaged over the time interval required to complete 1 pitch. You can then compare data for each pitch rotation to see if a “steady state” has been achieved, or if the flow is still developing. 4. Click Next.Interface Definition is displayed. 5. Click Next.Boundary Definition is displayed. 6. Click Next.Final Operations is displayed. 7. Ensure that Operation is set to Enter General Mode. 8. Click Finish. Initial values are required, but will be supplied later using a results file.Setting Output Control 1. Click Output Control. 2. Click the Trn Results tab. 3. Create a new transient result with the name Transient Results 1. 4. Apply the following settings to Transient Results 1 Setting Value OptionSelected Variables Output Variables List * Pressure, Velocity, Velocity in Stn Frame Output Frequency > Option Time Interval Output Frequency > Time Interval2.124e-5 [s]*.Use the key to select more than one variable. 5. Click OK.Writing the Solver (.def) File 1. Click Write Solver File .Page 218ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.230. Tutorial 12: Flow in an Axial Rotor/Stator: Obtaining a Solution to the Transient Rotor-Stator Model A warning will appear, due to a lack of initial values. 2. Click Yes.Initial values are required, but will be supplied later using a results file. 3. Apply the following settings:Setting ValueFile name Axial.defQuit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 4. Ensure Start Solver Manager is selected and click Save. 5. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution to the Transient Rotor-Stator Model When the ANSYS CFX-Solver Manager has started you will need to specify an initial values file before starting the ANSYS CFX-Solver.Serial Solution If you do not have a license, or do not want to run ANSYS CFX in parallel, you can run it in serial. Solution time in serial is similar to the first part of this tutorial. 1. Under Initial Values File, click Browse . 2. Select AxialIni_001.res. 3. Click Open. 4. Click Start Run. 5. You may see a notice that the mesh from the initial values file will be used. This mesh isthe same as in the definition file. Click OK to continue.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed. 6. Click Yes to post-process the results when the completion message appears at the endof the run. 7. If using Standalone Mode, quit ANSYS CFX-Solver Manager. When you are finished, continue with Monitoring the Run (p. 220).Parallel Solution You can solve this example using either local parallel or distributed parallel, in the same way as in the first part of this tutorial. For details, see Obtaining a Solution to the Frozen Rotor Model (p. 214).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 219Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.231. Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Transient Rotor-Stator Results in ANSYS CFX-PostMonitoring the RunDuring the solution, look for the additional information that is provided for transientrotor-stator runs. Each time the rotor is rotated to its next position, the number of degreesof rotation and the fraction of a pitch moved is given. You should see that after 10 timestepsthe rotor has been moved through 1 pitch.Viewing the Transient Rotor-Stator Results in ANSYS CFX-PostTo examine the transient interaction between the rotor and stator, you are going to createa blade-to-blade animation of pressure. A turbo surface will be used as the basis for this plot.Initializing Turbo-Post1. Click the Turbo tab. The Turbo Initialization dialog box is displayed, and asks you whether you want to auto-initialize all components.Note: If you do not see the Turbo Initialization dialog box, or as an alternative to using thatdialog box, you can initialize all components by clicking the Initialize All Componentsbutton which is visible initially by default, or after double-clicking the Initialization objectin the Turbo tree view.2. Click Yes. Both components (domains) are now being initialized based on the automatically selected turbo regions. When the process is complete, a green turbine icon appears next to each component entry in the list. Also, the viewer displays a green background mesh for each initialized component.3. Double-click Component 1 (S1) and review the automatically-selected turbo regions.Displaying a Surface of Constant Span1. In the Turbo tree view, double-click Blade-to-Blade.A surface of constant span appears, colored by pressure. This object can be edited andthen redisplayed using the details view.Using Multiple Turbo Viewports1. In the Turbo tree view, double-click Initialization.2. Click Three Views. Left view is 3D View, top right is Blade-to-Blade and bottom right is Meridional view.3. Click Single View.Creating a Turbo Surface Midway Between the Hub and Shroud1. Create a Turbo Surface from the Insert drop down menu with a Constant Span and value of 0.5.Page 220 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.232. Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post 2. Under the Color panel select Variable and set it to Pressure with a user specified rangeof -10000 [Pa] to -7000 [Pa].Setting up Instancing Transformations Next, you will use instancing transformations to view a larger section of the model. The properties for each domain have already been entered during the initialization phase, so only the number of instances needs to be set. 1. In the Turbo tree view, double-click the 3D View object. 2. In the Instancing section of the form, set # of Copies to 6 for R1. 3. Click Apply. 4. In the Instancing section of the form, set # of Copies to 6 for S1. 5. Click Apply. 6. Return to the Outline tab and ensure that the turbo surface is visible again.Creating a Transient Animation Start by loading the first timestep: 1. Click Timestep Selector. 2. Select time value 0. 3. Click Apply to load the timestep.The rotor blades move to their starting position. This is exactly 1 pitch from the previousposition so the blades will not appear to move. 4. Clear Visibility for Wireframe. 5. Position the geometry as shown below, ready for the animation. During the animationthe rotor blades will move to the right. Make sure you have at least two rotor blades outof view to the left side of the viewer. They will come into view during the animation. 6. In the toolbar at the top of the window click Animation. 7. In the Animation dialog box, click Newto create KeyFrameNo1. 8. Highlight KeyframeNo1, then set # of Frames to 9. 9. Use the Timestep Selector to load the final timestep.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 221Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.233. Tutorial 12: Flow in an Axial Rotor/Stator: Viewing the Transient Rotor-Stator Results in ANSYS CFX-Post10. In the Animation dialog box, click Newto create KeyframeNo2.11. Click More Animation Optionsto expand the Animation dialog box.12. Click Options and set Transient Case to TimeValue Interpolation. Click OK.The animation now contains a total of 11 frames (9 intermediate frames plus the twoKeyframes), one for each of the available time values.13. In the expanded Animation dialog box, select Save MPEG.14. Click Browse, next to the Save MPEG box and then set the file name to anappropriate file name.15. If frame 1 is not loaded (shown in the F: text box at the bottom of the Animation dialogbox), click To Beginningto load it.Wait for ANSYS CFX-Post to finish loading the objects for this frame before proceeding.16. Click Play the animation .•It takes a while for the animation to complete.•To view the MPEG file, you will need to use a media player that supports the MPEG format.You will be able to see from the animation, and from the plots created previously, thatthe flow is not continuous across the interface. This is because a pitch change occurs.The relatively coarse mesh and the small number of timesteps used in the transientsimulation also contribute to this. The movie was created with a narrow pressure rangecompared to the global range which exaggerates the differences across the interface.Further PostprocessingYou can use the Turbo Calculator to produce a report on the performance of the turbine.1. Edit the Gas Turbine Performance macro in the Turbo tree view.2. Set Ref Radius to 0.4575 and leave other settings at their default values.3. Click Calculate.4. Click View Report.Page 222 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.234. Tutorial 13:Reacting Flow in a Mixing TubeIntroduction This tutorial includes: • Tutorial 13 Features (p. 223) • Overview of the Problem to Solve (p. 224) • Outline of the Process (p. 224) • Defining a Simulation in ANSYS CFX-Pre (p. 225) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 237) • Viewing the Results in ANSYS CFX-Post (p. 237) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 225). Sample files referenced by this tutorial include: • Reactor.pre • ReactorExpressions.ccl • ReactorMesh.gtmTutorial 13 Features This tutorial addresses the following features of ANSYS CFX.ANSYS CFX TutorialsPage 223ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.235. Tutorial 13: Reacting Flow in a Mixing Tube: Overview of the Problem to Solve Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeVariable Composition Mixture Domain Type Single Domain Turbulence Modelk-Epsilon Heat Transfer Thermal Energy Particle Tracking Component Source Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Symmetry Plane Wall: Adiabatic Additional Variables CEL (CFX Expression Language) TimestepPhysical Time Scale ANSYS CFX-PostPlots Isosurface Slice Plane Other Changing the Color RangeIn this tutorial you will learn about:• Creating and using a multicomponent fluid in ANSYS CFX-Pre.• Using CEL to model a reaction in ANSYS CFX-Pre.• Using an algebraic additional variable to model a scalar distribution.• Using a subdomain as the basis for component sources.Overview of the Problem to SolveReaction engineering is one of the main core components in the chemical industry.Optimizing reactor design leads to higher yields, lower costs and, as a result, higher profit.This example demonstrates the capability of ANSYS CFX in modeling basic reacting flowsusing a multicomponent fluid model.Outline of the ProcessThe model is a mixing tube into which acid and alkali are injected through side holes. Thereaction to be modeled is: H 2 SO 4 + 2NaOH → Na 2 SO 4 + 2H 2 O (Eqn. 1)The tube is modeled as an axisymmetric section.Page 224 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.236. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-Pre The reaction between acid and alkali is represented as a single step irreversible liquid-phase reaction A+B→C(Eqn. 2) Reagent A (dilute sulphuric acid) is injected through a ring of holes near the start of the tube. As it flows along the tube it reacts with Reagent B (dilute sodium hydroxide) which is injected through a further two rings of holes downstream. The product, C , remains in solution. The composition and pH of the mixture within the tube are principal quantities of interest to be predicted by the model. The flow is assumed to be fully turbulent and turbulence is assumed to have a significant effect on the process. The process is also exothermic.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: Reactor.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 237).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type Reactor. 6. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 225Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.237. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-Pre Setting Value File name ReactorMesh.gtm 3. Click Open.Creating a Multicomponent Fluid In addition to providing template fluids, ANSYS CFX allows you to create custom fluids for use in all your ANSYS CFX models. These fluids may be defined as a pure substance, but may also be defined as a mixture, consisting of a number of transported fluid components. This type of fluid model is useful for applications involving mixtures, reactions, and combustion. In order to define custom fluids, ANSYS CFX-Pre provides the Material details view. This tool allows you to define your own fluids as pure substances, fixed composition mixtures or variable composition mixtures using a range of template property sets defined for common materials. The mixing tube application requires a fluid made up from four separate materials (or components). The components are the reactants and products of a simple chemical reaction together with a neutral carrier liquid. You are first going to define the materials that take part in the reaction (acid, alkali and product) as pure substances. The neutral carrier liquid is water; this material is already defined since it is commonly used. Finally, you will create a variable composition mixture consisting of these four materials. This is the fluid that you will use in your simulation. A variable composition mixture (as opposed to a fixed composition mixture) is required because the proportion of each component will change throughout the simulation due to the reaction.Acid properties1. Create a new material named acid. 2. Apply the following settings TabSetting Value Basic Settings OptionPure SubstanceThermodynamic State (Selected)Thermodynamic State > Thermodynamic State LiquidPage 226ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.238. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTabSetting ValueMaterial PropertiesThermodynamic Properties > Equation of State 19.52 [kg kmol^-1]* > Molar Mass Thermodynamic Properties > Equation of State 1080 [kg m^-3] > Density Thermodynamic Properties > Specific Heat(Selected) Capacity Thermodynamic Properties > Specific Heat4190 [J kg^-1 K^-1] Capacity > Specific Heat Capacity Transport Properties > Dynamic Viscosity(Selected) Transport Properties > Dynamic Viscosity >Value Option Transport Properties > Dynamic Viscosity >0.001 [kg m^-1 s^-1] Dynamic Viscosity Transport Properties > Thermal Conductivity (Selected) Transport Properties > Thermal Conductivity > 0.6 [W m^-1 K^-1] Thermal Conductivity *.The Molar Masses for the three materials created are only set for completeness since they are not used when solving this problem. 3. Click OK.Alkali 1. Create a new material named alkali.properties 2. Apply the following settingsTabSetting ValueBasic Settings OptionPure Substance Thermodynamic State (Selected) Thermodynamic State > Thermodynamic State LiquidMaterial PropertiesThermodynamic Properties > Equation of State 20.42 [kg kmol^-1] > Molar Mass Thermodynamic Properties > Equation of State 1130 [kg m^-3] > Density Thermodynamic Properties > Specific Heat(Selected) Capacity Thermodynamic Properties > Specific Heat4190 [J kg^-1 K^-1] Capacity > Specific Heat Capacity Transport Properties > Dynamic Viscosity(Selected) Transport Properties > Dynamic Viscosity >0.001 [kg m^-1 s^-1] Dynamic Viscosity Transport Properties > Thermal Conductivity (Selected) Transport Properties > Thermal Conductivity > 0.6 [W m^-1 K^-1] Thermal Conductivity 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 227Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.239. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreProduct of the1. Create a new material named product.reaction2. Apply the following settingspropertiesTabSetting ValueBasic Settings OptionPure Substance Thermodynamic State (Selected) Thermodynamic State > Thermodynamic State LiquidMaterial PropertiesThermodynamic Properties > Equation of State 21.51 [kg kmol^-1] > Molar Mass Thermodynamic Properties > Equation of State 1190 [kg m^-3] > Density Thermodynamic Properties > Specific Heat(Selected) Capacity Thermodynamic Properties > Specific Heat4190 [J kg^-1 K^-1] Capacity > Specific Heat Capacity Transport Properties > Dynamic Viscosity(Selected) Transport Properties > Dynamic Viscosity >0.001 [kg m^-1 s^-1] Dynamic Viscosity Transport Properties > Thermal Conductivity (Selected) Transport Properties > Thermal Conductivity > 0.6 [W m^-1 K^-1] Thermal Conductivity3. Click OK.Fluid properties1. Create a new material named mixture.2. Apply the following settingsTabSetting ValueBasic Settings OptionVariable Composition Mixture Material GroupUser, Water Data Materials ListWater, acid, alkali, product Thermodynamic State (Selected) Thermodynamic State > Liquid Thermodynamic State3. Click OK.Creating an Additional Variable to Model pHYou are going to use an additional variable to model the distribution of pH in the mixingtube. You can create additional variables and use them in selected fluids in your domain.1. Create a new additional variable named MixturePH.2. Apply the following settingsPage 228 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.240. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBasic SettingsUnits [kg kg^-1] 3. Click OK. This additional variable is now available for use when you create or modify a domain.Defining the Reaction Reactions and reaction kinetics can be modeled using CFX Expression Language (CEL), together with appropriate settings for Component sources. This section shows you how to develop an Eddy Break Up (EBU) type term using CEL to simulate the reaction between acid and alkali.Reaction SourceThe reaction and reaction rate are modeled using a basic Eddy Break Up formulation for theTermscomponent and energy sources, so that, for example, the transport equation for mass fraction of acid is∂ d ---- ( ρm f acid ) + ∇•( ρU mf acid ) – ∇ • ( ρD A ∇m f acid )- ∂t(Eqn. 3)εmf alkali = – 4ρ --min ⎛ mf acid, ---------------- ⎞-k ⎝i ⎠ where mf is mass fraction, D A is the kinematic diffusivity (set above) and i is the stoichiometric ratio. The right hand side represents the source term applied to the transport equation for the mass fraction of acid. The left hand side consists of the transient, advection and diffusion terms. For acid-alkali reactions, the stoichiometric ratio is usually based on volume fractions. To correctly model the reaction using an Eddy Break Up formulation based on mass fractions, you must calculate the stoichiometric ratio based on mass fractions. In this tutorial the reaction is modeled by introducing source terms for the acid, alkali and product components. You can now also model this type of flow more easily using a reacting mixture as your fluid. There is also a tutorial example using a reacting mixture. For details, see Tutorial 18: Combustion and Radiation in a Can Combustor (p. 299). Technical Note (Reference Only) In ANSYS CFX, Release 11.0, a source is fully specified by an expression for its value S. A source coefficient C is optional, but can be specified to provide convergence enhancement or stability for strongly-varying sources. The value of C may affect the rate of convergence but should not affect the converged results.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 229Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.241. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreIf no suitable value is available for C , the solution time scale or timestep can still be reducedto help improve convergence of difficult source terms.Important: C must never be positive.An optimal value for C when solving an individual equation for a positive variable φ with asource S whose strength decreases with increasing φ is∂S C = (Eqn. 4)∂φWhere this derivative cannot be computed easily, S C = ---(Eqn. 5) φmay be sufficient to ensure convergence.Another useful recipe for C is ρ C = – ---(Eqn. 6) τwhere τ is a local estimate for the source time scale. Provided that the source time scale isnot excessively short compared to flow or mixing time scales, this may be a useful approachfor controlling sources with positive feedback ( ∂S ⁄ ∂φ > 0 ) or sources that do not dependdirectly on the solved variable φ .Calculating pHThe pH (or acidity) of the mixture is a function of the mass fraction of acid, alkali and product.For the purposes of this calculation, acid is assumed to be dilute and fully dissociated into+ -its respective ions ( H and X ); alkali is assumed to be dilute and fully dissociated into its +-respective ions ( Y and OH ); product is assumed to be a salt solution including further+- H and OH ions in a stoichiometric ratio.The concentrations of hydrogen and hydroxyl ions can be calculated from the massfractions of the components using the following expressions: mf prod [ H ] acid = αρ ⎛ mf acid + --------------- ⎞ = [ X ]+ i–i - (Eqn. 7) ⎝1+i ⎠imf prod [ OH ] alkali = βρ ⎛ mf alkali + ----------------- ⎞ = [ Y ] - i+i-(Eqn. 8)⎝ 1+i ⎠Page 230 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.242. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-Pre - + where α and β are the X ion and Y ion concentrations in the acid and alkali- respectively. For this problem, α is set to 1.0E-05 kmole X per kg of acid, and β = α ⁄ i . Applying charge conservation and equilibrium conditions,+ +- - [ H ] + [ Y ] = [ X ] + [ OH ] (Eqn. 9)+ - [ H ] [ OH ] = K W(Eqn. 10) gives the following quadratic equation for free hydrogen ion concentration:+ ++ - [ H ] ( [ H ] + [ Y ] –[ X ] ) = K W(Eqn. 11)+ 2 +- + [H ] + ([Y ] – [X ])[H ] – K W = 0(Eqn. 12)i+i pH = – log 10 [ H ] (Eqn. 13) where K W is the equilibrium constant (1.0 x 10E-14 kmoles2 m-6).+ The quadratic equation can be solved for [ H ] using the equation 2+– b + b – 4ac+ - [ H ] = ------------------------------------- where a = 1 , b = [ Y ] – [ X ] and c = – K W . - 2aCreating You can create the expressions required to model the reaction sources and pH by eitherexpressions to reading them in from a file or by defining them in the Expressions workspace. Note that themodel the expressions used here do not refer to a particular fluid since there is only a single fluid. In areaction multiphase simulation you must prefix variables with a fluid name, for example Mixture.acid.mf instead of acid.mf. In this tutorial the expressions can be imported from a file to avoid typing them.Reading1. Select File > Import CCL.expressions2. Ensure that Import Method is set to Append.from a file 3. Select ReactorExpressions.ccl, which should be in your working directory. 4. Click Open. Note that the expressions have been loaded.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 231Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.243. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTabSetting ValueGeneralBasic Settings > Domain TypeFluid DomainOptions Basic Settings > Fluids Listmixture Domain Models > Pressure > Reference Pressure 1 [atm]Fluid Models Heat Transfer > OptionThermal Energy Component Details acid Component Details > acid > Option Transport Equation Component Details > acid > Kinematic Diffusivity(Selected) Component Details > acid > Kinematic Diffusivity > 0.001 [m^2 s^-1] Kinematic Diffusivity3. Use the same Option and Kinematic Diffusivity settings for alkali and product as you have just set for acid.4. For Water, set Option to Constraint as followsTabSetting ValueFluid Models Component Details Water Component Details > Water > OptionConstraintOne component must always use Constraint. This is the component used to balancethe mass fraction equation; the sum of the mass fractions of all components of a fluidmust equal unity.5. Apply the following settingsTabSetting ValueFluid Models Additional Variable Details > MixturePH (Selected) Additional Variable Details > MixturePH > Algebraic Equation Option Additional Variable Details > MixturePH > pH Value6. Click OK.Creating a Subdomain to Model the Chemical ReactionsTo provide the correct modeling for the chemical reaction you need to define sources forthe fluid components acid, alkali ,and product. To do this, you need to create asubdomain where the relevant sources can be specified. In this case, sources need to beprovided within the entire domain of the mixing tube since the reaction occurs throughoutthe domain.1. Create a new subdomain named sources.2. Apply the following settingsPage 232 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.244. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTab Setting ValueSources Sources (Selected)Sources > Equation Sourcesacid.mfSources > Equation Sources > acid.mf(Selected)Sources > Equation Sources > acid.mf > Source AcidSourceSources > Equation Sources > acid.mf > Source Coefficient (Selected)Sources > Equation Sources > acid.mf > Source Coefficient > AcidSourceCoeffSource CoefficientSources > Equation Sourcesalkali.mfSources > Equation Sources > alkali.mf(Selected)Sources > Equation Sources > alkali.mf > Source AlkaliSourceSources > Equation Sources > alkali.mf > Source Coefficient (Selected)Sources > Equation Sources > alkali.mf > Source Coefficient > AlkaliSourceCoeffSource CoefficientSources > Equation SourcesEnergySources > Equation Sources > Energy (Selected)Sources > Equation Sources > Energy > SourceHeatSourceSources > Equation Sourcesproduct.mfSources > Equation Sources > product.mf (Selected)Sources > Equation Sources > product.mf > SourceProductSourceSources > Equation Sources > product.mf > Source Coefficient (Selected)Sources > Equation Sources > product.mf > Source Coefficient 0 [kg m^-3 s^-1]> Source Coefficient 3. Click OK.Creating the Boundary ConditionsWater Inlet1. Create a new boundary condition named InWater.Boundary 2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation InWaterBoundary DetailsMass and Momentum > Normal Speed 2 [m s^-1]Heat Transfer > Option Static TemperatureHeat Transfer > Static Temperature 300 [K] 3. Leave mass fractions for all components set to zero. Since Water is the constraint fluid,it will be automatically given a mass fraction of 1 on this inlet. 4. Click OK.Acid Inlet 1. Create a new boundary condition named InAcid.BoundaryANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 233Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.245. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-Pre2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation InAcidBoundary DetailsMass and Momentum > Normal Speed 2 [m s^-1]Heat Transfer > Option Static TemperatureHeat Transfer > Static Temperature 300 [K]Component DetailsacidComponent Details > acid > Mass Fraction 1.0Component DetailsalkaliComponent Details > alkali > Mass Fraction 0Component DetailsproductComponent Details > product > Mass Fraction03. Click OK.Alkali InletThe inlet area for the alkali is twice that of the acid and it also enters at a higher velocity. TheBoundaryresult is an acid-to-alkali volume inflow ratio of 1:2.667. Recall that a stoichiometric ratio of2.7905 was specified based on mass fractions. When the density of the acid (1080 [kg m^3])and alkali (1130 [kg m^3]) are considered, the acid-to-alkali mass flow ratio can becalculated as 1:2.7905. You are therefore providing enough acid and alkali to produce aneutral solution if they react together completely.1. Create a new boundary condition named InAlkali.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation InAlkaliBoundary DetailsMass and Momentum > Normal Speed 2.667 [m s^-1]Heat Transfer > Option Static TemperatureHeat Transfer > Static Temperature 300 [K]Component Details > acid (Selected)Component Details > acid > Mass Fraction 0Component Details > alkali (Selected)Component Details > alkali > Mass Fraction 1Component Details > product(Selected)Component Details > product > Mass Fraction03. Click OK.Outlet1. Create a new boundary condition named out.Boundary2. Apply the following settingsPage 234 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.246. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBasic SettingsBoundary Type OutletLocationoutBoundary DetailsMass and Momentum > OptionStatic PressureMass and Momentum > Relative Pressure 0 [Pa] 3. Click OK.Symmetry 1. Create a new boundary condition named sym1.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type SymmetryLocationsym1 3. Click OK. 4. Create a new boundary condition named sym2. 5. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type SymmetryLocationsym2 6. Click OK. The default adiabatic wall boundary condition will automatically be applied to the remaining unspecified boundary.Setting Initial Values The values for acid, alkali and product will be initialized to 0. Since Water is the constrained component, it will make up the remaining mass fraction which, in this case, is 1. 1. Click Global Initialization . 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 235Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.247. Tutorial 13: Reacting Flow in a Mixing Tube: Defining a Simulation in ANSYS CFX-PreTabSettingValueGlobal Initial Conditions > Cartesian Velocity Components > Automatic with ValueSettings Option Initial Conditions > Cartesian Velocity Components > U 2 [m s^-1] Initial Conditions > Cartesian Velocity Components > V 0 [m s^-1] Initial Conditions > Cartesian Velocity Components > W 0 [m s^-1] Initial Conditions > Turbulence Eddy Dissipation (Selected) Initial Conditions > Turbulence Eddy Dissipation > Automatic Option Initial Conditions > Component Details acid Initial Conditions > Component Details > acid > Option Automatic with Value Initial Conditions > Component Details > acid > Mass 0 Fraction Initial Conditions > Component Details alkali Initial Conditions > Component Details > alkali > Option Automatic with Value Initial Conditions > Component Details > alkali > Mass 0 Fraction Initial Conditions > Component Details product Initial Conditions > Component Details > product > Automatic with Value Option Initial Conditions > Component Details > product > Mass 0 Fraction3. Click OK.Setting Solver Control1. Click Solver Control.2. Apply the following settingsTab SettingValueBasic SettingsAdvection Scheme > OptionSpecific Blend FactorAdvection Scheme > Blend Factor0.75Convergence Control > Max. Iterations50Convergence Control > Fluid TimescalePhysical TimescaleControl > Timescale ControlConvergence Control > Fluid Timescale0.01 [s]*Control > Physical Timescale *.The length of mixing tube is 0.06 [m] and inlet velocity is 2 [m s^-1]. An estimate of the dynamic time scale is 0.03 [s]. An appropriate timestep would be 1/4 to 1/2 of this value.Page 236 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.248. Tutorial 13: Reacting Flow in a Mixing Tube: Obtaining a Solution using ANSYS CFX-Solver Manager 3. Click OK. Note: At this point, you might see a physics validation message regarding a change in the advection scheme. This change will not affect the outcome of the simulation; you will still be able to run this simulation in the ANSYS CFX-Solver.Writing the Solver (.def) File 1. Click Write Solver File . 2. Apply the following settings:Setting ValueFile name Reactor.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager When the ANSYS CFX-Solver Manager has started, obtain a solution to the CFD problem by following the instructions below. Using the double precision ANSYS CFX-Solver executable is recommended for this case: 1. Ensure Define Run is displayed. 2. Select Show Advanced Controls. On the Solver tab, select Double Precision underExecutable Settings. 3. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed. 4. Click Yes to post-process the results. 5. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-Post Try the following: • Create an XY plane through Z = 0 colored by MixturePH. The lower and upper bounds depend on the precision setting used in the ANSYS CFX-Solver should approximately range from 2 to 15 (single) or 2 to 11 (double).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 237Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.249. Tutorial 13: Reacting Flow in a Mixing Tube: Viewing the Results in ANSYS CFX-PostFigure 1 shows two planes colored by MixturePH, with the plane on the right having amore accurate solution throughout the domain.Figure 1 Comparison of Single and Double Precision Results for pH Variance• View the acid, alkali and product mass fractions on the same plane.• Create isosurfaces of Turbulence Kinetic Energy and Turbulence EddyDissipation.Page 238 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.250. Tutorial 14:Conjugate Heat Transfer in aHeating CoilIntroduction This tutorial includes: • Tutorial 14 Features (p. 240) • Overview of the Problem to Solve (p. 241) • Defining a Simulation in ANSYS CFX-Pre (p. 241) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 246) • Viewing the Results in ANSYS CFX-Post (p. 246) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 241). Sample files referenced by this tutorial include: • HeatingCoil.pre • HeatingCoil_001.res • HeatingCoilMesh.gtmANSYS CFX TutorialsPage 239ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.251. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Tutorial 14 FeaturesTutorial 14 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateFluid TypeGeneral FluidDomain Type Multiple DomainTurbulence Modelk-EpsilonHeat Transfer Thermal EnergyConjugate Heat TransferSubdomainsEnergy SourceBoundary Conditions Inlet (Subsonic)OpeningWall: No-SlipWall: AdiabaticCEL (CFX Expression Language)TimestepPhysical Time ScaleANSYS CFX-PostPlots CylinderDefault LocatorsIsosurfaceOther Changing the Color RangeExpression Details ViewLighting AdjustmentVariable Details View In this tutorial you will learn about: • Creating and using a solid domain as a heater coil in ANSYS CFX-Pre. • Modeling conjugate heat transfer in ANSYS CFX-Pre. • Specifying a subdomain to specify a heat source. • Creating a cylinder locator using CEL in ANSYS CFX-Post. • Examining the temperature distribution which is affected by heat transfer from the coil to the fluid.Page 240ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.252. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Overview of the Problem to SolveOverview of the Problem to Solve This example demonstrates the capability of ANSYS CFX in modeling conjugate heat transfer. In this example, part of the model of a simple heat exchanger is used to model the transfer of heat from a solid to a fluid. The model consists of a fluid domain and a solid domain. The fluid domain is an annular region through which water flows at a constant rate. The heater is a solid copper coil modeled as a constant heat source.Outflow Solid Heater Inflow This tutorial also includes an optional step that demonstrates the use of the CFX to ANSYS Data Transfer Tool to export thermal and mechanical stress data for analysis in ANSYS. A results file is provided in case you wish to skip the model creation and solution steps within ANSYS CFX.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: HeatingCoil.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 246).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type HeatingCoil.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 241Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.253. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Defining a Simulation in ANSYS CFX-Pre6. Click Save.Importing the Mesh1. Right-click Mesh and select Import Mesh.2. Apply the following settingsSetting ValueFile name HeatingCoilMesh.gtm3. Click Open.4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.Creating the DomainsThis simulation requires both a fluid and a solid domain. First, you will create a fluid domainfor the annular region of the heat exchanger.Creating a FluidThe fluid domain will include the region of fluid flow but exclude the solid copper heater.Domain1. Click Domainand set the name to FluidZone.2. Apply the following settings to FluidZoneTabSetting ValueGeneralBasic Settings > Location B1.P3*Options Basic Settings > Fluids ListWater Domain Models > Pressure > Reference Pressure 1 [atm]Fluid Models Heat Transfer > OptionThermal EnergyInitialization Domain Initialization (Selected) Domain Initialization > Initial Conditions(Selected) Domain Initialization > Initial Conditions > Turbulence (Selected) Eddy Dissipation *.This region name may be different depending on how the mesh was created. You should pick the region that forms the exterior surface of the volume surrounding the coil.3. Click OK.Creating a SolidSince you know that the copper heating element will be much hotter than the fluid, you canDomaininitialize the temperature to a reasonable value. The initialization option that is set whencreating a domain applies only to that domain.1. Create a new domain named SolidZone.2. Apply the following settingsPage 242 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.254. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Defining a Simulation in ANSYS CFX-PreTab SettingValueGeneral Basic Settings > LocationB2.P3OptionsBasic Settings > Domain Type Solid DomainBasic Settings > Solids List CopperSolid ModelsHeat Transfer > Option Thermal EnergyInitializationDomain Initialization(Selected)Domain Initialization > Initial Conditions (Selected)Domain Initialization > Initial Conditions > Automatic withTemperature > Option ValueDomain Initialization > Initial Conditions > 550 [K]Temperature > Temperature 3. Click OK.Creating a Subdomain to Specify a Thermal Energy Source To allow a thermal energy source to be specified for the copper heating element, you need to create a subdomain. 1. Create a new subdomain named Heater in the domain SolidZone. 2. Apply the following settingsTab SettingValueBasic SettingsBasic Settings > LocationB2.P3*Sources Sources(Selected)Sources > Equation Sources > Energy(Selected)Sources > Equation Sources > Energy > Source 1.0E+07 [W m^-3] *.This is the same location as for the domain SolidZone, because you want the source term to apply to the entire solid domain. 3. Click OK.Creating the Boundary ConditionsInlet Boundary You will now create an inlet boundary condition for the cooling fluid (Water). 1. Create a new boundary condition named inflow in the domain FluidZone. 2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation inflowBoundary DetailsMass and Momentum > Normal Speed 0.4 [m s^-1]Heat Transfer > Static Temperature 300 [K] 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 243Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.255. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Defining a Simulation in ANSYS CFX-PreOpening The opening boundary condition type is used in this case because at some stage during theboundarysolution, the coiled heating element will cause some recirculation at the exit. At an openingboundary you need to set the temperature of fluid that enters through the boundary. In thiscase it is useful to base this temperature on the fluid temperature at the outlet, since youexpect the fluid to be flowing mostly out through this opening.1. Create a new expression named OutletTemperature.2. Set Definition to areaAve(T)@REGION:outflow3. Click Apply.4. Create a new boundary condition named outflow in the domain FluidZone.5. Apply the following settings:Tab SettingValueBasic SettingsBoundary TypeOpeningLocation outflowBoundary DetailsMass and Momentum > Option Opening Pres. and DirnMass and Momentum > Relative Pressure0 [Pa]Heat Transfer > Option Static TemperatureHeat Transfer > Static Temperature OutletTemperature6. Click OK.The default adiabatic wall boundary condition will automatically be applied to theremaining unspecified external boundaries of the fluid domain. The default Fluid-SolidInterface boundary condition (flux conserved) will be applied to the surfaces betweenthe solid domain and the fluid domain.Creating the Domain InterfaceIf you have the Generate Default Domain Interfaces option turned on (from Edit >Options > CFX-Pre), then you will see that an interface calledDefault Fluid Solid Interface already exists, and is listed in the Outline tree view. Ifthis is the case, you can optionally skip the following instructions for creating a domaininterface (since the domain interface set here will have the same settings as, and willautomatically replace, the default domain interface).If you have the Generate Default Domain Interfaces option turned off, then there is nodomain interface defined at this point. In this case, create a domain interface using eitherone of the following methods (the result is the same):Creating a1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDefault Domain Interfaces is selected. An interface named Default Fluid Solid Interface shouldInterface now appear under the Simulation branch.Creating a1. Double click Default Fluid Solid Interface and apply the following settings:DomainInterfaceManuallyPage 244 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.256. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic SettingsInterface Type Fluid SolidInterface Side 1 > Domain (Filter) FluidZoneInterface Side 1 > Region List F10.B1.P3, F5.B1.P3, F6.B1.P3, F7.B1.P3, F8.B1.P3, F9.B1.P3Interface Side 2 > Domain (Filter) SolidZoneInterface Side 2 > Region List F10.B2.P3, F5.B2.P3, F6.B2.P3, F7.B2.P3, F8.B2.P3, F9.B2.P3Interface Models > OptionGeneral ConnectionInterface Models > Frame Change/Mixing NoneModel > OptionInterface Models > Pitch Change > Option NoneMesh Connection Method > OptionAutomatic 2. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settings:Tab SettingValueBasic SettingsConvergence Control > Fluid TimescalePhysical TimescaleControl > Timescale ControlConvergence Control >Fluid Timescale 2 [s]Control > Physical Timescale For the Convergence Criteria, an RMS value of at least 1e-05 is usually required for adequate convergence, but the default value is sufficient for demonstration purposes. 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settings:Setting ValueFile name HeatingCoil.defQuit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 245Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.257. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Obtaining a Solution using ANSYS CFX-Solver Manager4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a Solution using ANSYS CFX-Solver ManagerWhile the calculations proceed, you can see residual output for various equations in boththe text area and the plot area. Use the tabs to switch between different plots (e.g., HeatTransfer, Turbulence Quantities, etc.) in the plot area. You can view residual plots for thefluid and solid domains separately by editing the Workspace Properties.1. Ensure Define Run is displayed.2. Click Start Run. ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long time depending on your system. Eventually a dialog box is displayed.3. Click Yes to post-process the results.4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-PostThe following topics will be discussed:• Creating a Cylindrical Locator (p. 246)• Specular Lighting (p. 247)• Moving the Light Source (p. 247)Creating a Cylindrical LocatorNext, you will create a cylindrical locator close to the outside wall of the annular domain.This can be done by using an expression to specify radius and locating a particular radiuswith an isosurface.Expression1. Create a new expression named expradius.2. Apply the following settingsSetting ValueDefinition(x^2 + y^2)^0.53. Click Apply.Variable1. Create a new variable named radius.2. Apply the following settingsSetting ValueExpressionexpradiusPage 246 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.258. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Exporting the Results to ANSYS 3. Click Apply.Isosurface of the 1. Create a new isosurface named Isosurface 1.variable2. Apply the following settingsTab Setting ValueGeometryDefinition > Variable radiusDefinition > Value0.8 [m]*Color ModeVariableVariableTemperatureRange User SpecifiedMin 300 [K]Max 302 [K]RenderDraw Faces(Selected) *.The maximum radius is 1 m, so a cylinder locator at a radius of 0.8 m is suitable. 3. Click Apply.Specular Lighting Specular lighting is on by default. Specular lighting allows glaring bright spots on the surface of an object, depending on the orientation of the surface and the position of the light. 1. Apply the following settings to Isosurface 1Tab Setting ValueRenderDraw Faces > Specular (Cleared) 2. Click Apply.Moving the Light Source To move the light source, click within the 3-D Viewer, then press and hold while pressing the arrow keys left, right, up or down. Tip: If using the Standalone version, you can move the light source by positioning the mouse pointer in the viewer, holding down the key, and dragging using the right mouse button.Exporting the Results to ANSYS This optional step involves generating an ANSYS .cdb data file from the results generated in ANSYS CFX-Solver. The .cdb file could then be used with the ANSYS Multi-field solver to measure the combined effects of thermal and mechanical stresses on the solid heating coil. There are two possible ways to export data to ANSYS:ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 247Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.259. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Exporting the Results to ANSYS• Use ANSYS CFX-Solver Manager to export data. For details, see Exporting Data fromANSYS CFX-Solver Manager (p. 248).• Use ANSYS CFX-Post to export data. This involves:a. Importing a surface mesh from ANSYS into ANSYS CFX-Post, and associating the surface with the corresponding 2D region in the ANSYS CFX-Solver results file.b. Exporting the data to a file containing SFE commands that represent surface element thermal or mechanical stress values.c. Loading the commands created in the previous step into ANSYS and visualizing the loads.Exporting Data from ANSYS CFX-Solver ManagerSince the heat transfer in the solid domain was calculated in ANSYS CFX, the 3D thermal datawill be exported to ANSYS Element Type as 3D Thermal (70) data. The mechanicalstresses are calculated on the liquid side of the liquid-solid interface. These values will beexported to ANSYS Element Type as 2D Stress (154) data.Thermal Data1. Start ANSYS CFX-Solver Manager.2. Select Tools > Export to ANSYS MultiField. Export to ANSYS MultiField Solver dialog box appears.3. Apply the following settings:SettingValueResults File HeatingCoil_001.resExport FileHeatingCoil_001_ansysfsi_70.csvDomain Name > Domain SolidZoneDomain Name > Boundary**Export Options > ANSYS Element Type3D Thermal (70) *.Leave Boundary empty.4. Click Export.When the export is complete, click OK to acknowledge the message and continue withthe next steps to export data for Mechanical Stresses.Mechanical1. Apply the following settings in the Export to ANSYS MultiField Solver dialog box (seeStresses Step 2 above):SettingValueResults File HeatingCoil_001.resExport FileHeatingCoil_001_ansysfsi_154.csvDomain Name > Domain FluidZoneDomain Name > Boundary FluidZone DefaultExport Options > ANSYS Element Type2D Stress (154)2. Click Export.Page 248 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.260. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Exporting the Results to ANSYS You now have two exported files that can be loaded into ANSYS Multiphysics. When you are finished, close ANSYS CFX-Solver Manager and ANSYS CFX-Post.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 249Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.261. Tutorial 14: Conjugate Heat Transfer in a Heating Coil: Exporting the Results to ANSYSPage 250 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.262. Tutorial 15:Multiphase Flow in MixingVesselIntroduction This tutorial includes: • Tutorial 15 Features (p. 252) • Overview of the Problem to Solve (p. 253) • Defining a Simulation in ANSYS CFX-Pre (p. 253) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 265) • Viewing the Results in ANSYS CFX-Post (p. 265) If this is the first tutorial you are working with it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 253). Sample files referenced by this tutorial include: • MixerImpellerMesh.gtm • MixerTank.geo • MultiphaseMixer.preANSYS CFX TutorialsPage 251ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.263. Tutorial 15: Multiphase Flow in Mixing Vessel: Tutorial 15 FeaturesTutorial 15 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateFluid TypeGeneral FluidDomain Type Multiple DomainRotating Frame of ReferenceTurbulence ModelDispersed Phase Zero EquationFluid-Dependant TurbulenceModelk-EpsilonHeat Transfer NoneBuoyant FlowMultiphaseBoundary Conditions Inlet (Subsonic)Outlet (Degassing)Wall: Thin SurfaceWall: (Slip Depends on VolumeFraction)Domain Interfaces Frozen RotorPeriodicOutput ControlTimestepPhysical Time ScaleANSYS CFX-PostPlots Default LocatorsIsosurfaceSlice PlaneOther Quantitative Calculation In this tutorial you will learn about: • Importing meshes that have CFX-4 and ANSYS CFX .def/.res file formats. • Setting up a simulation using multiple frames of reference. • Connecting two domains (one for the impeller and one for the tank) via Frozen Rotor interfaces. • Modeling rotational periodicity using periodic boundary conditions. • Using periodic GGI interfaces where the mesh does not map exactly. • Using thin surfaces for the blade and baffle surfaces. • Setting up a multiphase flow problem.Page 252ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.264. Tutorial 15: Multiphase Flow in Mixing Vessel: Overview of the Problem to SolveOverview of the Problem to Solve This example simulates the mixing of two fluids in a mixing vessel. The geometry consists of a mixing tank vessel containing four baffles. A rotating impeller blade is connected to a shaft which runs vertically through the vessel. Air is injected into the vessel through an inlet pipe located below the impeller blade at a speed of 5 m/s. Figure 1 Cut-away diagram of Mixing Vessel Shaft BafflesMixing TankAir Inlet Impeller The figure above shows the full geometry, with part of the tank walls and one baffle cut away. The symmetry of the vessel allows a 1/4 section of the full geometry to be modeled.Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: MultiphaseMixer.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 265).Creating a New Simulation 1. Start ANSYS CFX-Pre.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 253Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.265. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-Pre2. Select File > New Simulation.3. Select General and click OK.4. Select File > Save Simulation As.5. Under File name, type MultiphaseMixer.6. Click Save.Importing the MeshesIn this tutorial, a CFX-4 mesh is imported using advanced options. These options controlhow the CFX-4 mesh is imported into ANSYS CFX.By creating 3D regions on fluid regions, you prevent import of USER3D and POROUS regions.Turn off this option if you do not need these regions for sub-domains. This will simplify theregions available in ANSYS CFX-Pre. In this case, the mesh file contains USER3D regions thatwere created as a location for a thin surface and you do not need them for defining anysubdomains.Importing the 1. Right-click Mesh and select Import Mesh.Mixer Tank2. Apply the following settingsMeshSettingValueFile typeCFX-4 (*geo)File nameMixerTank.geoAdvanced Options > Create 3D Regions on > Fluid Regions(Cleared)(USER3D, POROUS)3. Click Open.Importing the 1. Right-click Mesh and select Import Mesh to import the second mesh.Impeller Mesh 2. Apply the following settingsSettingValueFile typeCFX Mesh (*gtm)File nameMixerImpellerMesh.gtm3. Click Open.4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (X up) to view the mesh assemblies.TransformingIn the next step you will move the impeller mesh to its correct position.the Impeller1. Right-click MixerImpellerMesh.gtm and select Transform Mesh.Mesh The Mesh Transformation Editor dialog box appears.2. Apply the following settingsPage 254 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.266. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreTab SettingValueDefinitionTransformation TranslationApply Translation > Method DeltasApply Translation > Dx, Dy, Dz 0.275, 0, 0 3. Click OK.Viewing the1. Click Label and Marker Visibility .Mesh at the2. Apply the following settingTank PeriodicBoundaryTab SettingValueLabel Options Show Labels(Cleared) 3. Click OK. 4. In the Outline workspace, expand MixerImpellerMesh.gtm and MixerTank.geo toview associated 2D primitives. 5. Under MixerTank.geo > Principal 3D regions > Primitive 3D, click the primitiveregion BLKBDY_TANK_PER2. You can now see the mesh on one of the periodic regions of the tank. To reduce the solution time for this tutorial, the mesh used is very coarse. This is not a suitable mesh to obtain accurate results, but it is sufficient for demonstration purposes. Note: If you do not see the surface mesh, highlighting may be turned off. If highlighting is disabled, toggle Highlight. The default highlight type will show the surface mesh for any selected regions. If you see a different highlighting type, you can alter it by selecting Edit > Options and browsing to CFX-Pre > Viewer.Creating the DomainsRotating 1. Click Domainand set the name to impeller.Domain for the 2. Apply the following settingsImpellerANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 255Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.267. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreTabSetting ValueGeneralBasic Settings > Location MainOptions Basic Settings > Fluids ListAir at 25 C, Water Domain Models > Pressure > Reference Pressure 1 [atm] Domain Models > Buoyancy > Option Buoyant Domain Models > Buoyancy > Gravity X Dirn.-9.81 [m s^-2] Domain Models > Buoyancy > Gravity Y Dirn.0 [m s^-2] Domain Models > Buoyancy > Gravity Z Dirn.0 [m s^-2] Domain Models > Buoyancy > Buoy. Ref. Density*997 [kg m^-3] Domain Models > Domain Motion > OptionRotating Domain Models > Domain Motion > Angular Velocity84 [rev min-1]† Domain Models > Domain Motion > Axis Definition > Global X Rotation AxisFluidMultiphase Options > Homogeneous Model(Cleared)Models Multiphase Options > Allow Musig Fluids (Cleared) Multiphase Options > Free Surface Model > OptionNone Heat Transfer > Homogeneous Model (Cleared) Heat Transfer > OptionIsothermal Heat Transfer > Fluid Temperature 25 [C] Turbulence > Homogeneous Model(Cleared) Turbulence > Option Fluid DependentFluidFluid Details Air at 25 CDetails Fluid Details > Air at 25 C > Morphology > Option Dispersed Fluid Fluid Details > Air at 25 C > Morphology > Mean Diameter3 [mm]FluidFluid Pairs Air at 25 C | WaterPairsFluid Pairs > Air at 25 C | Water > Surface Tension Coefficient (Selected) Fluid Pairs > Air at 25 C | Water > Surface Tension Coefficient 0.073 [N m^-1]‡ > Surf. Tension Coeff. Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag Grace Force > Option Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag (Selected) Force > Volume Fraction Correction Exponent Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag 4 Force > Volume Fraction Correction Exponent > Value Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Lopez de Non-drag forces > Turbulent Dispersion Force > Option Bertodano Fluid Pairs > Air at 25 C | Water > Momentum Transfer > 0.1 Non-drag forces > Turbulent Dispersion Force > Dispersion Coeff. Fluid Pairs > Air at 25 C | Water > Turbulence Transfer > Sato Enhanced OptionEddy ViscosityPage 256 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.268. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-Pre *.For dilute dispersed multiphase flow, always set the buoyancy reference density to that for continuous fluid. †.Note the unit. ‡.This must be set to allow the Grace drag model to be used. 3. Click OK.Stationary Next, you will create a stationary domain for the main tank by copying the properties of theDomain for the existing fluid domain.Main Tank 1. Right-click impeller and select Duplicate from the shortcut menu. 2. Set the name of this domain to tank and open it for editing. 3. Apply the following settingsTab Setting ValueGeneral Options Basic Settings > Location Primitive 3DDomain Models > Domain Motion > StationaryOption 4. Click OK.Creating the Boundary Conditions The following boundary conditions that define the problem will be set: • An inlet through which air enters the mixer. • A degassing outlet, so that only the gas phase can leave the domain. • Thin surfaces for the baffle and impeller blade. • A wall for the hub and shaft in the rotating domain. This will be stationary relative to the rotating domain. • A wall for the shaft in the stationary domain. This will be rotating relative to the stationary domain. • Periodic domain interfaces for the periodic faces of the tank and impeller. Periodic domain interfaces can either be one-to-one or GGI interfaces. One-to-one transformations occur for topologically similar meshes whose nodes match within a given tolerance. One-to-one periodic interfaces are more accurate and reduce CPU and memory requirements. When the default wall boundary condition is generated, the internal 2D regions of an imported mesh are ignored, while the regions that form domain boundaries are included.Air Inlet1. Create a new boundary condition in the domain tank named Airin.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type InletLocationINLET_DIPTUBEBoundary DetailsMass and Momentum > OptionFluid DependentANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 257Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.269. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreTab SettingValueFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Velocity 5 [m s^-1]> Normal SpeedBoundary Conditions > Air at 25 C > Volume 1Fraction > Volume FractionBoundary ConditionsWaterBoundary Conditions > Water > Velocity > 5 [m s^-1]Normal SpeedBoundary Conditions > Water > Volume 0Fraction > Volume Fraction3. Click OK.Degassing 1. Create a new boundary condition in the domain tank named LiquidSurface.Outlet2. Apply the following settingsBoundaryTab SettingValueBasic SettingsBoundary TypeOutletLocation WALL_LIQUID_SURFACEBoundary DetailsMass and Momentum > Option Degassing Condition3. Click OK.Thin Surface forIn ANSYS CFX-Pre, thin surfaces can be created by specifying wall boundary conditions onthe Baffleboth sides of internal 2D regions. Both sides of the baffle regions will be specified as walls inthis case.1. Create a new boundary condition in the domain tank named Baffle.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeWallLocation WALL_BAFFLES*Boundary DetailsWall Influence On Flow > OptionFluid DependentFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall Free SlipInfluence on Flow > OptionBoundary ConditionsWaterBoundary Conditions > Water > Wall No Slip†Influence on Flow > Option *.The WALL_BAFFLES region includes the surfaces on both sides of the baffle (you can confirm this by examining WALL_BAFFLES in the region selector). Therefore, you do not need to use the Create Thin Surface Partner option. †.The Free Slip condition can be used for the gas phase since the contact area with the walls is near zero for low gas phase volume fractions.3. Click OK.Page 258 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.270. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreWall BoundaryThe next stage involves setting up a boundary condition for the shaft, which exists in theCondition fortank (stationary domain). These regions are connected to the shaft in the impeller domain.the Shaft Since the tank domain is not rotating, you need to specify a moving wall to account for the rotation of the shaft. Part of the shaft is located directly above the air inlet, so the volume fraction of air in this location will be high and the assumption of zero contact area for the gas phase is not physically correct. In this case, a no slip boundary condition is more appropriate than a free slip condition for the air phase. When the volume fraction of air in contact with a wall is low, a free slip condition is more appropriate for the air phase. In cases where it is important to correctly model the dispersed phase slip properties at walls for all volume fractions, you can declare both fluids as no slip, but set up an expression for the dispersed phase wall area fraction. The expression should result in an area fraction of zero for dispersed phase volume fractions from 0 to 0.3, for example, and then linearly increase to an area fraction of 1 as the volume fraction increases to 1. 1. Create a new boundary condition in the domain tank named TankShaft. 2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeWallLocation WALL_SHAFT, WALL_SHAFT_CENTERBoundary DetailsWall Influence On Flow > OptionFluid DependentFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall No SlipInfluence on Flow > OptionBoundary Conditions > Air at 25 C > Wall (Selected)Influence on Flow > Wall VelocityBoundary Conditions > Air at 25 C > Wall Rotating WallInfluence on Flow > Wall Velocity > OptionBoundary Conditions > Air at 25 C > Wall84 [rev min-1]*Influence on Flow > Wall Velocity > AngularVelocityBoundary Conditions > Air at 25 C > Wall Global XInfluence on Flow > Wall Velocity > AxisDefinition > Rotation Axis *.Note the unit. 3. Select Water and set the same values as for Air at 25 C. 4. Click OK.Required 1. Create a new boundary condition in the domain impeller named Blade.Boundary 2. Apply the following settingsConditions inthe ImpellerDomainANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 259Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.271. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic SettingsBoundary TypeWallLocation BladeThin Surfaces > Create Thin Surface Partner (Selected)*Boundary DetailsWall Influence On Flow > OptionFluid DependentFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall Free SlipInfluence on Flow > OptionBoundary ConditionsWaterBoundary Conditions > Water > Wall No SlipInfluence on Flow > Option *.The Blade region only includes the surface from one side of the blade (you can confirm this by examining Blade in the region selector). Therefore, you can select Create Thin Surface Partner to include the surfaces from the other side of the blade.3. Click OK. You will see in the tree view that a boundary named Blade Other Side has automatically been created.4. Create a new boundary condition in the domain impeller named HubShaft.5. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeWallLocation Hub, ShaftBoundary DetailsWall Influence On Flow > OptionFluid DependentFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall Free SlipInfluence on Flow > OptionBoundary ConditionsWaterBoundary Conditions > Water > Wall No SlipInfluence on Flow > Option6. Click OK.Modifying the 1. On the tree view, open tank Default for editing.Default Wall2. Apply the following settingsBoundaryConditionTab SettingValueBoundary DetailsWall Influence On Flow > OptionFluid DependentPage 260 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.272. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreTab SettingValueFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall Free SlipInfluence on Flow > OptionBoundary ConditionsWaterBoundary Conditions > Water > Wall No SlipInfluence on Flow > Option 3. Click OK. It is not necessary to set the default boundary in the impeller domain since the remaining surfaces will be assigned interface conditions in the next section.Creating the Domain InterfacesImpeller 1. Create a new domain interface named ImpellerPeriodic.Domain 2. Apply the following settingsTab SettingValueBasic SettingsInterface Type Fluid FluidInterface Side 1 > Domain (Filter) impellerInterface Side 1 > Region List Periodic1Interface Side 2 > Domain (Filter) impellerInterface Side 2 > Region List Periodic2Interface Models > OptionRotational PeriodicityInterface Models > Axis Definition > Global XRotation Axis 3. Click OK.Tank Domain1. Create a new domain interface named TankPeriodic. 2. Apply the following settingsTab SettingValueBasic SettingsInterface Type Fluid FluidInterface Side 1 > Domain (Filter) tankInterface Side 1 > Region List BLKBDY_TANK_PER1Interface Side 2 > Domain (Filter) tankInterface Side 2 > Region List BLKBDY_TANK_PER2Interface Models > OptionRotational PeriodicityInterface Models > Axis Definition > Global XRotation Axis 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 261Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.273. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreFrozen RotorNext, you will create three Frozen Rotor interfaces for the regions connecting the twoInterface domains. In this case three separate interfaces are created. You should not try to create asingle domain interface for multiple surfaces that lie in different planes.1. Create a new domain interface named Top.2. Apply the following settingsTab SettingValueBasic SettingsInterface Type Fluid FluidInterface Side 1 > Domain (Filter) impellerInterface Side 1 > Region List TopInterface Side 2 > Domain (Filter) tankInterface Side 2 > Region List BLKBDY_TANK_TOPInterface Models > Frame Change/Mixing Frozen RotorModel > Option3. Click OK.4. Create a new domain interface named Bottom.5. Apply the following settingsTab SettingValueBasic SettingsInterface Type Fluid FluidInterface Side 1 > Domain (Filter) impellerInterface Side 1 > Region List BottomInterface Side 2 > Domain (Filter) tankInterface Side 2 > Region List BLKBDY_TANK_BOTInterface Models > Frame Change/Mixing Frozen RotorModel > Option6. Click OK.7. Create a new domain interface named Outer.8. Apply the following settingsTab SettingValueBasic SettingsInterface Type Fluid FluidInterface Side 1 > Domain (Filter) impellerInterface Side 1 > Region List OuterInterface Side 2 > Domain (Filter) tankInterface Side 2 > Region List BLKBDY_TANK_OUTERInterface Models > Frame Change/Mixing Frozen RotorModel > Option9. Click OK.Page 262 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.274. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreSetting Initial Values The initialization for volume fraction is 0 for air and automatic for water. Therefore, the initial volume fraction for water will be set to 1 so that the sum of the two fluid volume fractions is 1. It is important to understand how the velocity is initialized in this tutorial. Here, both fluids use Automatic for the Cartesian Velocity Components. When the Automatic option is used, the initial velocity field will be based on the velocity values set at inlets, openings, and outlets. In this tutorial, the only boundary that has a set velocity value is the inlet, which specifies a velocity of 5 [m s^-1] for both phases. Without setting the Velocity Scale parameter, the resulting initial guess would be a uniform velocity of 5 [m s^-1] in the X-direction throughout the domains for both phases. This is clearly not suitable since the water phase is enclosed by the tank. When the boundary velocity conditions are not representative of the expected domain velocities, the Velocity Scale parameter should be used to set a representative domain velocity. In this case the velocity scale for water is set to zero, causing the initial velocity for the water to be zero. The velocity scale is not set for air, resulting in an initial velocity of 5 [m s^-1] in the X-direction for the air. This should not be a problem since the initial volume fraction of the air is zero everywhere. 1. Click Global Initialization . 2. Apply the following settingsTab Setting ValueFluid SettingsFluid Specific Initialization Air at 25 CFluid Specific Initialization > Air at 25 C > Initial Automatic with ValueConditions > Volume Fraction > OptionFluid Specific Initialization > Air at 25 C > Initial 0Conditions > Volume Fraction > Volume FractionFluid Specific Initialization WaterFluid Specific Initialization > Water > Initial (Selected)Conditions > Cartesian Velocity Components >Velocity ScaleFluid Specific Initialization > Water > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components >Velocity Scale > ValueFluid Specific Initialization > Water > Initial (Selected)Conditions > Turbulence Eddy Dissipation 3. Click OK.Setting Solver Control Generally, two different time scales exist for multiphase mixers. The first is a small time scale based on the rotational speed of the impeller, typically taken as 1 / ω , resulting in a time scale of 0.11 s for this case. The second time scale is usually larger and based on the recirculation time of the continuous phase in the mixer.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 263Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.275. Tutorial 15: Multiphase Flow in Mixing Vessel: Defining a Simulation in ANSYS CFX-PreUsing a timestep based on the rotational speed of the impeller will be more robust, butconvergence will be slow since it takes time for the flow field in the mixer to develop. Usinga larger timestep reduces the number of iterations required for the mixer flow field todevelop, but reduces robustness. You will need to experiment to find an optimum timestep.Note: You may find it useful to monitor the value of an expression during the solver run sothat you can view the volume fraction of air in the tank (the gas hold up). The gas hold up isoften used to judge convergence in these types of simulations by converging until asteady-state value is achieved. You could create the following expressions:TankAirHoldUp = volumeAve(Air at 25 C.vf)@tankImpellerAirHoldUp = volumeAve(Air at 25 C.vf)@impellerTotalAirHoldUp = (volume()@tank * TankAirHoldUp + volume()@impeller *ImpellerAirHoldUp) / (volume()@tank + volume()@impeller)and then monitor the value of TotalAirHoldUp.1. Click Solver Control.2. Apply the following settingsTab SettingValueBasic SettingsConvergence Control > Fluid TimescalePhysical TimescaleControl > Timescale ControlConvergence Control > Fluid Timescale2 [s]*Control > Physical Timescale *.This is an aggressive timestep for this case.3. Click OK.Setting Output ControlIn the next step, you will choose to write additional data to the results file which allows forceand torque calculations to be performed in post-processing.1. Click Output Control.2. Apply the following settingsTab SettingValueResults Output Boundary Flows(Selected)Output Boundary Flows > Boundary Flows All3. Click OK.Writing the Solver (.def) FileSince this tutorial uses domain interfaces and you choose to summarize the interface data,an information window is displayed that informs you of the connection type used for eachdomain interface.1. Click Write Solver File .2. Apply the following settings:Page 264 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.276. Tutorial 15: Multiphase Flow in Mixing Vessel: Obtaining a Solution using ANSYS CFX-Solver Manager SettingValue File nameMultiphaseMixer.def Summarize Interface Data (Selected) Quit CFX–Pre*(Cleared)*. If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save.If you are notified the file already exists, click Overwrite.A message about interface connections appears. 4. Click OK. 5. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre has closed down. You will be able to obtain a solution to the CFD problem by following the instructions below. 1. Ensure Define Run is displayed. 2. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system.After a run has finished, examine some of the information printed at the end of the OUTfile.A common quantity of interest is the mass balance; this compares the amount of fluidleaving the domain to the amount entering. •You usually want the Global Imbalance, in %: to be less than 0.1 % in a convergedsolution. •For a single phase calculation, the mass balance is the P-Mass equation. •For a multiphase calculation, examine the information given for the P-Vol equation. •This is not the volumetric flow balance information, but is the summation of thephasic continuity mass balance information. 3. Click Yes to post-process the results when the completion message appears at the endof the run. 4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-Post When ANSYS CFX-Post has started you will be able to see the mixer geometry in the Viewer. You will create some plots showing how effective mixing has occurred. You will also calculate the torque and power required by the impeller.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 265Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.277. Tutorial 15: Multiphase Flow in Mixing Vessel: Viewing the Results in ANSYS CFX-PostVisualizing the Mixing ProcessCreating a plane 1. Create a new plane named Plane 1.2. Apply the following settingsTab SettingValueGeometryDefinition > MethodThree PointsDefinition > Point 1 1, 0, 0Definition > Point 2 0, 1, -0.9Definition > Point 3 0, 0, 0Color Mode VariableVariable Air at 25 C.Volume FractionRangeUser SpecifiedMin0Max0.043. Click Apply.4. Observe the plane, then apply the following settings:Tab SettingValueColor Variable Air at 25 C.Shear Strain RateRangeUser SpecifiedMin0 [s^-1]Max15 [s^-1]5. Click Apply. Areas of high shear strain rate or shear stress are typically also areas where the highest mixing occurs.6. Observe the plane, then apply the following settings:Tab SettingValueColor Variable PressureRangeLocal7. Click Apply.Note that the hydrostatic contribution to pressure is excluded due to the use of anappropriate buoyancy reference density. If you plot the variable called AbsolutePressure, you will see the true pressure including the hydrostatic contribution.Creating a1. Create a new vector named Vector 1.vector2. Apply the following settingsPage 266 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.278. Tutorial 15: Multiphase Flow in Mixing Vessel: Viewing the Results in ANSYS CFX-PostTab SettingValueGeometryDefinition > Locations Plane 1Variable Water.Velocity in Stn Frame*SymbolSymbol Size0.2Normalize Symbols(Selected) *.Using this variable, instead of Water.Velocity, results in the velocity vectors appearing to be continuous at the interface between the rotating and stationary domains. Velocity variables that do not include a frame specification always use the local reference frame. 3. Observe the vector plot, then change the variable to Air at 25 C.Velocity in StnFrame. Observe this as well, then clear the visibility of Vector 1. 4. Modify the tank Default object. 5. Apply the following settings:Tab SettingValueColor Mode VariableVariable Water.Wall ShearRangeLocal The legend for this plot shows the range of wall shear values. The global maximum wall shear is much higher than the maximum value on the default walls. The global maximum values occur on the TankShaft boundary directly above the inlet. Although these values are very high, the shear force exerted on this boundary will be small since the contact area fraction of water here is very small.Calculating1. Select Tools > Function Calculator from the main menu or click Show FunctionPower and Calculator from the main toolbar.TorqueRequired by the2. Apply the following settings:ImpellerTab SettingValueFunctionFunction torqueCalculatorLocation BladeAxis Global XFluidAll Fluids 3. Click Calculate to find the torque required to rotate Blade about the X-axis. 4. Repeat the calculation setting Location to Blade Other Side. The sum of these two results is the torque required by the single impeller blade, approximately 70 [N m]. This must be multiplied by the number of blades in the full geometry to obtain the total torque required by the impeller; the result is a value of approximately 282 [N m]. You could also include the results from the locations HubShaft and TankShaft; however in this case their contributions are negligible.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 267Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.279. Tutorial 15: Multiphase Flow in Mixing Vessel: Viewing the Results in ANSYS CFX-PostThe power requirement is simply the required torque multiplied by the rotational speed(8.8 rad/s): Power = 282*8.8 = 2482 [W].Remember that this value is the power requirement for the work done on the fluid only, itdoes not account for any mechanical losses, efficiencies etc. Also note that the accuracy ofthese results is significantly affected by the coarseness of the mesh. You should not use amesh of this length scale to obtain accurate quantitative results.Page 268 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.280. Tutorial 16:Gas-Liquid Flow in an AirliftReactorIntroduction This tutorial includes: • Tutorial 16 Features (p. 270) • Overview of the Problem to Solve (p. 270) • Defining a Simulation in ANSYS CFX-Pre (p. 271) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 277) • Viewing the Results in ANSYS CFX-Post (p. 278) • Additional Fine Mesh Simulation Results (p. 280) If this is the first tutorial you are working with it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 271). Sample files referenced by this tutorial include: • BubbleColumn.pre • BubbleColumnMesh.gtmANSYS CFX TutorialsPage 269ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.281. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Tutorial 16 FeaturesTutorial 16 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode GeneralSimulation Type Steady StateFluid TypeGeneral FluidDomain Type Single DomainTurbulence ModelDispersed Phase Zero EquationFluid-Dependent TurbulenceModelk-EpsilonHeat Transfer NoneBuoyant FlowMultiphaseBoundary Conditions Inlet (Subsonic)Outlet (Degassing)Symmetry PlaneWall: Thin SurfaceWall: (Slip Depends on VolumeFraction)TimestepPhysical Time ScaleANSYS CFX-PostPlots Default LocatorsVectorOther Changing the Color RangeSymmetry In this tutorial you will learn about: • Setting up a multiphase flow involving air and water • Using a fluid dependent turbulence model to set different turbulence options for each fluid. • Specifying buoyant flow. • Specifying a degassing outlet boundary condition to allow air, but not water, to escape from the boundary.Overview of the Problem to Solve This tutorial demonstrates the Eulerian–Eulerian multiphase model in ANSYS CFX. The tutorial simulates a bubble column with an internal tube (draft tube) used to direct recirculation of the flow. This configuration is known as an airlift reactor. Bubble columns are tall gas-liquid contacting vessels and are often used in processes where gas absorption is important (e.g., bioreactors to dissolve oxygen in broths) and to limit the exposure of micro-organisms to excessive shear, imparted by mechanically driven mixers.Page 270ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.282. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre This example models the dispersion of air bubbles in water. The gas is supplied through a sparger at the bottom of the vessel and the rising action of the bubbles provides gentle agitation of the liquid. Simple bubble columns that are without the draft tube tend to develop irregular flow patterns and poor overall mixing. The draft tube in the airlift reactor helps establish a regular flow pattern in the column and achieve better uniformity of temperature, concentration and pH in the liquid phase, but sometimes at the expense of decreased mass transfer from the gas to the liquid. This tutorial also demonstrates the use of thin surfaces. Thin surfaces are internal two dimensional wall boundaries used to model thin three dimensional features (e.g., baffles, guide vanes within ducts, etc.). The airlift reactor that is modeled here is very similar to the laboratory bench scale prototype used by García-Calvo and Letón. If you are interested, a formal analysis of this simulation involving a finer mesh is available at the end of this tutorial. For details, see Additional Fine Mesh Simulation Results (p. 280).Defining a Simulation in ANSYS CFX-Pre The following sections describe the simulation setup in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: BubbleColumn.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 277).Creating a New Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type BubbleColumn. 6. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 271Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.283. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre Setting Value File name BubbleColumnMesh.gtm 3. Click Open.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settings: TabSetting Value GeneralBasic Settings > Location B1.P3, B2.P3 OptionsBasic Settings > Fluids ListAir at 25 C, WaterDomain Models > Pressure > Reference Pressure 1 [atm]Domain Models > Buoyancy > Option BuoyantDomain Models > Buoyancy > Gravity X Dirn.0 [m s^-2]Domain Models > Buoyancy > Gravity Y Dirn.-9.81 [m s^-2]Domain Models > Buoyancy > Gravity Z Dirn.0 [m s^-2]Domain Models > Buoyancy > Buoy. Ref. Density*997 [kg m^-3] FluidMultiphase Options > Homogeneous Model(Cleared) ModelsMultiphase Options > Allow Musig Fluids (Cleared)Free Surface Model > Option NoneHeat Transfer > OptionIsothermalHeat Transfer > Fluid Temperature 25 CTurbulence > Option Fluid Dependent FluidFluid Details Air at 25 C DetailsFluid Details > Air at 25 C > Morphology > Option Dispersed FluidFluid Details > Air at 25 C > Morphology > Mean Diameter6 [mm]Page 272ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.284. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-PreTabSettingValueFluidFluid Pairs > Air at 25 C | Water > Surface Tension Coefficient (Selected)PairsFluid Pairs > Air at 25 C | Water > Surface Tension Coefficient 0.072 [N m^-1]† > Surf. Tension Coeff. Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag Grace Force > Option Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag (Selected) Force > Volume Fraction Correction Exponent Fluid Pairs > Air at 25 C | Water > Momentum Transfer > Drag 2 Force > Volume Fraction Correction Exponent > Value Fluid Pairs > Air at 25 C | Water > Momentum Transfer >Lopez de Non-drag Forces > Turbulent Dispersion Force > OptionBertodano Fluid Pairs > Air at 25 C | Water > Momentum Transfer >0.3 Non-drag Forces > Turbulent Dispersion Force > Dispersion Coeff. Fluid Pairs > Air at 25 C | Water > Turbulence Transfer >Sato Enhanced Option Eddy Viscosity *.For dilute dispersed multiphase flow, always set the buoyancy reference density to that for continuous fluid. †.This must be set to allow the Grace drag model to be used. 3. Click OK.Creating the Boundary Conditions For this simulation of the airlift reactor, the boundary conditions required are: • An inlet for air on the sparger. • A degassing outlet for air at the liquid surface. • A thin surface wall for the draft tube. • An exterior wall for the outer wall, base and sparger tube. • Symmetry planes for the cross sections.Inlet Boundary There are an infinite number of inlet velocity/volume fraction combinations that will produce the same mass inflow of air. The combination chosen gives an air inlet velocity close to the terminal rise velocity. Since the water inlet velocity is zero, you can adjust its volume fraction until the required mass flow rate of air is obtained for a given air inlet velocity. 1. Create a new boundary condition named Sparger. 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type InletLocationSpargerBoundary DetailsMass And Momentum > OptionFluid DependentANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 273Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.285. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre Tab SettingValue Fluid ValuesBoundary ConditionsAir at 25 C Boundary Conditions > Air at 25 C > Velocity 0.3 [m s^-1] > Normal Speed Boundary Conditions > Air at 25 C > Volume 0.25 Fraction > Volume Fraction Boundary ConditionsWater Boundary Conditions > Water > Velocity > 0 [m s^-1] Normal Speed Boundary Conditions > Water > Volume 0.75 Fraction > Volume Fraction 3. Click OK.Outlet The top of the reactor will be a degassing boundary, which is classified as an outletBoundary boundary. 1. Create a new boundary condition named Top. 2. Apply the following settings Tab SettingValue Basic SettingsBoundary TypeOutlet Location Top Boundary DetailsMass and Momentum > Option Degassing Condition 3. Click OK.Thin Surface Thin surfaces are created by specifying a wall boundary condition on both sides of anDraft Tube internal region. If only one side has a boundary condition then the ANSYS CFX-Solver willBoundary fail. To assist with this, you can select only one side of a thin surface and then enable the Create Thin Surface Partner toggle. ANSYS CFX-Pre will then try to automatically create another boundary condition for the other side. 1. Create a new boundary condition named DraftTube. 2. Apply the following settings Tab SettingValue Basic SettingsBoundary TypeWall Location Draft Tube Thin Surfaces > Create Thin Surface Partner (Selected) Boundary DetailsWall Influence On Flow > OptionFluid Dependent Fluid ValuesBoundary ConditionsAir at 25 C Boundary Conditions > Air at 25 C > Wall Free Slip Influence On Flow > Option Boundary ConditionsWater Boundary Conditions > Water > Wall No Slip Influence On Flow > OptionPage 274ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.286. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre 3. Click OK. A boundary condition named DraftTube Other Side will now be created automatically.Symmetry Plane In this step you will create symmetry plane boundary conditions on the Symmetry1 andBoundary Symmetry2 locators, one for each of the two vertical cross sections of the reactor sector. 1. Create a new boundary condition named SymP1. 2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeSymmetryLocation Symmetry1 3. Click OK. 4. Create a new boundary condition named SymP2. 5. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeSymmetryLocation Symmetry2 6. Click OK.Modifying theThe remaining external regions are assigned to the default wall boundary condition. ThisDefaultneeds to be modified to set the Air phase to Free Slip.Boundary 1. In the Outline workspace, open Default Domain Default for editing. 2. Apply the following settingsTab SettingValueBoundary DetailsWall Influence on Flow > OptionFluid DependentFluid ValuesBoundary ConditionsAir at 25 CBoundary Conditions > Air at 25 C > Wall Free SlipInfluence on Flow > Option 3. Click OK. The boundary condition specifications are now complete.Setting Initial Values It often helps to set an initial velocity for a dispersed phase that is different to that of the continuous phase. This results in a non-zero drag between the phases which can help stability at the start of a simulation. For some bubble column problems, improved convergence can be obtained by using CEL (CFX Expression Language) to specify a non zero volume fraction, for air in the riser and a zero value in the downcomer. This should be done if two solutions are possible (for example, if the flow could go up the downcomer and down the riser).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 275Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.287. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Defining a Simulation in ANSYS CFX-Pre 1. Click Global Initialization . Since a single pressure field exists for a multiphase calculation you do not set pressure values on a per fluid basis. 2. Apply the following settings TabSetting Value Fluid Settings Fluid Specific Initialization Air at 25 CFluid Specific Initialization > Air at 25 C (Selected)Fluid Specific Initialization > Air at 25 C > Initial Automatic with ValueConditions > Cartesian Velocity Components >OptionFluid Specific Initialization > Air at 25 C > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components > UFluid Specific Initialization > Air at 25 C > Initial 0.3 [m s^-1]Conditions > Cartesian Velocity Components > VFluid Specific Initialization > Air at 25 C > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components > WFluid Specific Initialization Water*Fluid Specific Initialization > Water (Selected)Fluid Specific Initialization > Water > Initial Automatic with ValueConditions > Cartesian Velocity Components >OptionFluid Specific Initialization > Water > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components > UFluid Specific Initialization > Water > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components > VFluid Specific Initialization > Water > Initial 0 [m s^-1]Conditions > Cartesian Velocity Components > WFluid Specific Initialization > Water > Initial AutomaticConditions > Turbulence Kinetic Energy > OptionFluid Specific Initialization > Water > Initial (Selected)Conditions > Turbulence Eddy DissipationFluid Specific Initialization > Water > Initial AutomaticConditions > Turbulence Eddy Dissipation >OptionFluid Specific Initialization > Water > Initial Automatic with ValueConditions > Volume Fraction > OptionFluid Specific Initialization > Water > Initial 1†Conditions > Volume Fraction > Volume Fraction*.Since there is no water entering or leaving the domain, a stationary initial guess isrecommended.†.The volume fractions must sum to unity over all fluids. Since a value has been set forwater, the volume fraction of air will be calculated as the remaining difference, inthis case, 0. 3. Click OK.Page 276ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.288. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Obtaining a Solution using ANSYS CFX-Solver ManagerSetting Solver Control If you are using a maximum edge length of 0.005 m or less to produce a finer mesh, use a Target Residual of 1.0E-05 to obtain a more accurate solution. 1. Click Solver Control . 2. Apply the following settingsTab SettingValueBasic SettingsConvergence Control > Fluid TimescalePhysical TimescaleControl > Timescale ControlConvergence Control > Fluid Timescale1 [s]Control > Physical Timescale 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settings:Setting ValueFile name BubbleColumn.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre has closed down. You will be able to obtain a solution to the CFD problem by following the instructions below. Note: If a fine mesh is used for a formal quantitative analysis of the flow in the reactor, the solution time will be significantly longer than for the coarse mesh. You can run the simulation in parallel to reduce the solution time. For details, see Obtaining a Solution in Parallel (p. 116). 1. Ensure Define Run is displayed. 2. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed stating that thesimulation has completed.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 277Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.289. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Viewing the Results in ANSYS CFX-Post 3. Click Yes to post-process the results when the completion message appears at the endof the run. 4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-Post The following topics will be discussed: • Creating Velocity Vector Plots (p. 278) • Viewing Volume Fractions (p. 279) • Displaying the Entire Airlift Reactor Geometry (p. 280)Creating Velocity Vector Plots Because the simulation in this tutorial is conducted on a coarse grid, the results are only suitable for a qualitative demonstration of the multiphase capability of ANSYS CFX, Release 11.0. You will first examine the distribution of velocities and fluid volume fraction by creating the following plots. The results will then be verified to check if the values are reasonable. 1. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z. 2. Zoom in as required. 3. Turn on the visibility of SymP1. 4. Apply the following settings to SymP1. Tab SettingValue Color Mode Variable Variable Air at 25 C.Volume Fraction RangeUser Specified Min0 Max0.025 5. Click Apply. Observe the volume fraction values throughout the domain. 6. Turn off the visibility of SymP1. 7. Create a new vector named Vector 1. 8. Apply the following settings Tab SettingValue GeometryDefinition > Locations SymP1 Definition > VariableWater.Velocity SymbolSymbol Size0.3 9. Click Apply. 10. Create a new vector plot named Vector 2.Page 278ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.290. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Viewing the Results in ANSYS CFX-Post 11. Apply the following settings TabSetting Value Geometry Definition > LocationsSymP1Definition > Variable Air at 25 C.Velocity Symbol Symbol Size 0.3 12. Click Apply. 13. Compare the vector fields by toggling the visibility of each and zooming in as needed.Viewing Volume Fractions In creating the geometry for the airlift reactor, a thin surface was used to model the draft tube. You will next plot the volume fraction of air on the thin surface. 1. Right-click on a blank area in the viewer, and select Predefined Camera > IsometricView (Y up). 2. Zoom in as required. 3. Turn off the visibility of any vector plots and turn on the visibility of DraftTube. 4. Modify DraftTube by applying the following settings TabSetting Value ColorModeVariableVariableAir at 25 C.Volume FractionRange User SpecifiedMin 0Max 0.02 5. Click Apply. •This boundary represents one side of the thin surface. When viewing plots on thinsurfaces, you must ensure that you are viewing the correct side of the thin surface. •The plot just created is displaying the volume fraction for air in the downcomerregion of the airlift reactor. If you rotate the geometry you will see that the same plotis visible from both sides of the thin surface. •You will make use of the face culling feature whichs turns off the visibility of the ploton one side of the thin surface. In this case, you need to turn off the “front” faces. 6. Modify DraftTube by applying the following settings TabSetting Value Render Draw Faces > Face Culling Front Faces 7. Click Apply. 8. Rotate the image in the viewer to see the effect of face culling on DraftTube. Youshould see that the color appears only on one side: the downcomer side. 9. Turn on the visibility of DraftTube Other Side.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 279Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.291. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Additional Fine Mesh Simulation Results 10. Color the DraftTube Other Side object using the same color settings as for DraftTube. Tab SettingValue Color Mode Variable Variable Air at 25 C.Volume Fraction RangeUser Specified Min0 Max0.02 11. Modify DraftTube Other Side by applying the following settings Tab SettingValue RenderDraw Faces > Face CullingFront Faces This will create a plot of air volume fraction on the riser side of the bubble column. 12. Click Apply. Rotating the geometry will now show correct plots of the air volume fraction on each side of the draft tube. To see why face culling was needed to prevent interference between the plots on each side of the draft tube, try turning off face culling for DraftTube and watch the effect on the riser side (Results may vary, which is why face culling was used to prevent interference.).Displaying the Entire Airlift Reactor Geometry Display the entire airlift reactor geometry by expanding User Locations and Plots and double-clicking the Default Transform object: 1. Apply the following settings to Default Transform Tab SettingValue DefinitionInstancing Info From Domain(Cleared) # of Copies12 Apply Rotation > AxisY Apply Rotation > # of Passages 12 2. Click Apply.Additional Fine Mesh Simulation Results A formal analysis of this airlift reactor was carried out on a finer grid (having 21000+ nodes and a maximum edge length of 0.005 m).Page 280ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.292. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Additional Fine Mesh Simulation Results The analysis showed a region of air bubble recirculation at the top of the reactor on the downcomer side. This was confirmed by zooming in on a vector plot of Air at 25 C.Velocity on SymP1 near the top of the downcomer. A similar plot of Water.Velocity revealed no recirculation of the water. Other results of the simulation: • Due to their large 0.006 m diameter, the air bubbles quickly attained a significant terminal slip velocity (i.e., the terminal velocity relative to water). The resulting terminal slip velocity, obtained using the Grace drag model, is consistent with the prediction by Maneri and Mendelson and the prediction by Baker and Chao. These correlations predict a terminal slip velocity of about 0.23 m s-1 to 0.25 m s-1 for air bubbles of the diameter specified. • The values of gas hold up (the average volume fraction of air in the riser), the superficial gas velocity (the rising velocity, relative to the reactor vessel, of gas bubbles in the riser, multiplied by the gas holdup), and the liquid velocity in the downcomer agree with the results reported by García-Calvo and Letón, for gas holdup values of 0.03 or less. At higher values of gas holdup, the multifluid model does not account for pressure-volume work transferred from gas to liquid due to isothermal expansion of the bubbles. The simulation therefore tends to under-predict both the superficial gas velocity in the riser, and the liquid velocity in the downcomer for gas holdup values greater than 0.03. Note: Multiphase results files contain the vector variable Fluid.Superficial Velocity defined as Fluid.Volume Fraction multiplied by Fluid.Velocity. This is sometimes also referred to as the fluid volume flux. The components of this vector variable are available as scalar variables (e.g., Fluid.Superficial Velocity X). Many reference texts on bubble columns cite the Hughmark correlation as a standard for gas hold up and superficial gas velocity in bubble columns. However, the Hughmark correlation should not be used when liquid flow is concurrent with gas at velocities exceeding 0.1 m s-1. In the airlift reactor described in this tutorial, the liquid velocity in the riser clearly exceeds 0.2 m s-1 and the Hughmark correlation is therefore not applicable.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 281Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.293. Tutorial 16: Gas-Liquid Flow in an Airlift Reactor: Additional Fine Mesh Simulation ResultsPage 282ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.294. Tutorial 17:Air Conditioning SimulationIntroduction This tutorial includes: • Tutorial 17 Features (p. 284) • Overview of the Problem to Solve (p. 285) • Defining a Simulation in ANSYS CFX-Pre (p. 285) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 295) • Viewing the Results in ANSYS CFX-Post (p. 295) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 285). Sample files referenced by this tutorial include: • HVAC.pre • HVAC_expressions.ccl • HVACMesh.gtm • TStat_Control.F Note: You must have a Fortran compiler installed on your system to perform this tutorial.ANSYS CFX TutorialsPage 283ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.295. Tutorial 17: Air Conditioning Simulation: Tutorial 17 FeaturesTutorial 17 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type TransientFluid TypeGeneral FluidDomain Type Single DomainTurbulence Modelk-EpsilonHeat Transfer Thermal EnergyRadiationBuoyant FlowBoundary Conditions Boundary Profile VisualizationInlet (Profile)Outlet (Subsonic)Wall: No-SlipWall: AdiabaticWall: Fixed TemperatureOutput ControlCEL (CFX Expression Language)User FortranTimestepTransient ExampleTransient Results FileANSYS CFX-PostPlots AnimationIsosurfacePointSlice PlaneOther Auto AnnotationChanging the Color RangeLegendMPEG GenerationTime Step SelectionTitle/TextTransient Animation In this tutorial you will learn about: • Using the Monte Carlo radiation model with a directional source of radiation. • Setting a monitor point to observe the temperature at a prescribed location.Page 284ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.296. Tutorial 17: Air Conditioning Simulation: Overview of the Problem to SolveOverview of the Problem to Solve This tutorial demonstrates a simple air conditioning case in a room. The room contains windows and an inlet vent for cooled air. The windows are set up to include heat and radiation sources that act to raise the temperature of the room. The inlet vent introduces cool air into the room to lower the temperature to a set level. The room also contains an outlet vent, which removes ambient air from the room.Roof Inlet Windows OutletDefining a Simulation in ANSYS CFX-Pre This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre. Important: You must have the required Fortran compiler installed and set in your system path in order to run this tutorial. For details on which Fortran compiler is required for your platform, see the applicable ANSYS, Inc. installation guide. If you are not sure which Fortran compiler is installed on your system, try running the cfx5mkext command (found in /bin) from the command line and read the output messages.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: HVAC.pre. After performing this step, you can continue from Obtaining a Solution using ANSYS CFX-Solver Manager (p. 295).ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 285Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.297. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-PreCreating a New Simulation1. Start ANSYS CFX-Pre.2. Select File > New Simulation.3. Select General and click OK.4. Select File > Save Simulation As.5. Under File name, type HVAC.6. Click Save.Importing the Mesh1. Right-click Mesh and select Import Mesh.2. Apply the following settingsSetting ValueFile name HVACMesh.gtm3. Click Open.4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.Creating ExpressionsThis tutorial requires some CEL expressions. In this tutorial, a transient simulation will beperformed over 3 minutes 45 seconds with 3 second timesteps for a total of 75 timesteps.Expressions will be used to enter these values. The expressions are also used to calculate theinlet temperature of air under different conditions.As the air conditioner will remove a specified amount of heat, the inlet vent temperature isa function of the outlet vent temperature. A CEL function is used to find the outlettemperature. A User CEL Function is used to simulate behavior of a thermostat that turns oncold air when the temperature (measured at a particular location) is above 22 °C (295.15 K)and turns off the cold air when the temperature falls below 20 °C (293.15 K).Note: The expression for TSensor requires a monitor point named Thermometer to provideroom temperature feedback to the thermostat. This will be set up later.Importing the 1. Select File > Import CCL.Expressions 2. Select the file HVAC_expressions.ccl.3. Click Open.The expression for ACOn requires a User CEL Function that indicates the thermostatoutput: whether the air conditioner should be on or off. This will be set up next.Page 286 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.298. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-PreInlet Velocity Expressions are used to simulate guiding vanes at the inlet, as the following diagram shows:ProfileFigure 1 Intended airflow direction from the roof inlet vent Roof Inlet Ventzx=0.15 x=0.05Wall x The two x locations indicated on the diagram correspond to the x values across the width of the inlet vent. When x is 0.05, the z component of velocity will be -1 and the x component will be zero. When x is 0.15, the x component of velocity will be 0.5 and the z component will be -0.5. The x component of velocity varies linearly with x. The following expression can be used to calculate the x component of velocity:x – 0.05 XCompInlet = 0.5 × ------------------ = 5 ( x – 0.05 )0.1 (Eqn. 1) ZCompInlet = – 1 + XCompInletSetting up the Thermostat A Fortran subroutine that simulates the thermostat has already been written for this tutorial.Compiling theYou can compile the subroutine and create the required library file used by ANSYSSubroutine CFX-Solver at any time before running the ANSYS CFX-Solver. The operation is performed at this point in the tutorial so that you have a better understanding of the values you need to specify in ANSYS CFX-Pre when creating a User CEL Function. The cfx5mkext command is used to compile the subroutine as described below. Important: You must have the required Fortran compiler installed and set in your system path in order to run the cfx5mkext command successfully. For details on which Fortran compiler is required for your platform, see the applicable ANSYS, Inc. installation guide. If you are not sure which Fortran compiler is installed on your system, try running the cfx5mkext command (found in /bin) from the command line and read the output messages. 1. Copy the subroutine TStat_Control.F to your working directory (if you have notalready done so). 2. Examine the contents of this file in any text editor to gain a better understanding of thissubroutine.This file was created by modifying the ucf_template.F file, which is available in the/examples/ directory.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 287Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.299. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-Pre3. Select Tools > Command Editor.4. Type the following command in the Command Editor dialog box (make sure you do not miss the semi-colon at the end of the line):! system (“cfx5mkext TStat_Control.F”) < 1 or die “cfx5mkext failed”;•This is equivalent to executing the following at an OS command prompt: cfx5mkext TStat_Control.F•The ! indicates that the following line is to be interpreted as power syntax and not CCL. Everything after the ! symbol is processed as Perl commands.•system is a Perl function to execute a system command.•The < 1 or die will cause an error message to be returned if, for some reason, there is an error in processing the command.5. Click Process to compile the subroutine.Note: You can use the -double option (i.e., cfx5mkext -double TStat_Control.F) tocompile the subroutine for use with double precision ANSYS CFX-Solver executables.A subdirectory will have been created in your working directory whose name is systemdependent (e.g., on IRIX it is named irix). This sub directory contains the shared objectlibrary.Note: If you are running problems in parallel over multiple platforms then you will need tocreate these subdirectories using the cfx5mkext command for each different platform.• You can view more details about the cfx5mkext command by runningcfx5mkext -help.• You can set a Library Name and Library Path using the -name and -dest optionsrespectively.• If these are not specified, the default Library Name is that of your Fortran file and thedefault Library Path is your current working directory.1. Close the Command Editor dialog box.Creating theA User CEL Function is required to link the subroutine into ANSYS CFX. The completeUser CELdefinition for the function is defined in two steps. First, a user routine that contains theFunctioncalling name, library name, and library path is created. Then, a user function that points tothe user routine, and also contains the argument and result units, is defined.1. From the main menu, select Insert > Expressions, Functions and Variables > UserRoutine or click User Routine.2. Set the name to Thermostat Routine.3. Apply the following settingsTabSetting ValueBasic Settings OptionUser CEL Function Calling Nameac_on* Library Name‘ TStat_Control† Library Path(Working Directory)‡Page 288 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.300. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-Pre *.This is the name of the subroutine within the Fortran file. Always use lower case letters for the calling name, even if the subroutine name in the Fortran file is in upper case. †.This is the name passed to the cfx5mkext command by the -name option. If the -name option is not specified, a default is used. The default is the Fortran file name without the .F extension. ‡.Set this to your working directory. 4. Click OK. 5. Create a new user function named Thermostat Function by selecting Insert >Expressions, Functions and Variables > User Function from the main menu. 6. Apply the following settingsTab Setting ValueBasic SettingsOptionUser FunctionArgument Units[K], [K], [K], []*Result Units[]† *.These are the units for the four input arguments: TSensor, TSet, TTol, and aitern. †.The result will be a dimensionless integer flag of values 1 or 0. 7. Click OK.The function you have just prepared is called during the evaluation of the expression forACOn (that you imported earlier). The expression is: Thermostat Function(TSensor,TSet,TTol,aitern) It evaluates to 1 or 0, depending on whether the air conditioner should be on (1) or off (0).Setting the Simulation Type 1. Click Simulation Type. 2. Apply the following settingsTab Setting ValueBasic SettingsSimulation Type > OptionTransientSimulation Type > Time Duration > Total TimetTotalSimulation Type > Time Steps > TimestepstStepSimulation Type > Initial Time > Time 0 [s] 3. Click OK.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settings:ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 289Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.301. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-PreTabSetting ValueGeneralBasic Settings > Location B1.P3Options Fluids List Air Ideal Gas Domain Models > Pressure > Reference Pressure 1 [atm] Domain Models > Buoyancy > Option Buoyant Domain Models > Buoyancy > Gravity X Dirn.0 [m s^-2] Domain Models > Buoyancy > Gravity Y Dirn.0 [m s^-2] Domain Models > Buoyancy > Gravity Z Dirn.-g Domain Models > Buoyancy > Buoy. Ref. Density 1.2 [kg m^-3]Fluid Models Heat Transfer > OptionThermal Energy Thermal Radiation Model > OptionMonte Carlo3. Click OK.Setting Boundary ConditionsIn this section you will define the locations and values of the boundary conditions.Inlet Boundary1. Create a new boundary condition named Inlet.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation InletBoundary DetailsMass and Momentum > Option Mass Flow RateMass and Momentum > Mass Flow Rate MassFlowFlow Direction > OptionCartesian ComponentsFlow Direction > X Component XCompInletFlow Direction > Y Component 0Flow Direction > Z Component ZCompInletHeat Transfer > Static Temperature TInPlot OptionsBoundary Vector(Selected)3. Click OK.Note: Ignore the physics errors that appear. They will be fixed by setting up the rest of thesimulation. The error you see is due to a reference to Thermometer which has not been setup yet. This will be done as part of the output control.Outlet1. Create a new boundary condition named VentOut.Boundary2. Apply the following settingsPage 290 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.302. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBasic SettingsBoundary Type OutletLocationVentOutBoundary DetailsMass and Momentum > Relative Pressure 0 [Pa] 3. Click OK.Window To model incoming radiation at the window boundaries, a directional radiation source willBoundary be created. The windows will also contribute heat to the room via a fixed temperature of 26 [C]. 1. Create a new boundary condition named Windows. 2. Apply the following settingsTabSettingValueBasicBoundary TypeWallSettings Location Window1, Window2Boundary Heat Transfer > Option TemperatureDetailsHeat Transfer > Fixed Temperature26 [C] 3. Apply the following settingsTabSettingValueSourcesBoundary Source(Selected) Boundary Source > Sources(Selected) 4. Create a new radiation source item by clicking Add New Itemand accepting thedefault name. 5. Apply the following settings to Radiation Source 1Setting ValueOptionDirectional Radiation FluxRadiation Flux600 [W m^-2]Direction > OptionCartesian ComponentsDirection > X Component 0.33Direction > Y Component 0.33Direction > Z Component -0.33 6. Apply the following settingTabSettingValuePlot Boundary Vector(Selected)OptionsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 291Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.303. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-Pre7. Click OK.The directional source of radiation is displayed.Default WallThe default boundary condition for any undefined surface in ANSYS CFX-Pre is a no-slip,Boundarysmooth, adiabatic wall. For radiation purposes, the default wall is assumed to be a perfectlyabsorbing and emitting surface (emissivity = 1), and this will be preserved when setting upthe boundary condition.In this tutorial, a fixed temperature of 26 °C will be assumed to exist at the wall during thesimulation. A more detailed analysis would model heat transfer through the walls, but asthis tutorial is designed only for demonstration purposes, a fixed temperature wall issufficient.1. Modify the boundary condition named Default Domain Default.2. Apply the following settingsTabSetting ValueBoundary Heat Transfer > OptionTemperatureDetailsHeat Transfer > Fixed Temperature 26 [C]3. Click OK.This setting will include the Door region, which will be modeled as a wall (closed door) forsimplicity. Since the region is part of the entire default boundary, it will not appear in thewireframe when the results file is opened in ANSYS CFX-Post (but can still be viewed in theRegions list).Setting Initial Values1. Click Global Initialization .2. Apply the following settingsPage 292 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.304. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-PreTab Setting ValueGlobal Settings Initial Conditions > Velocity TypeCartesianInitial Conditions > Cartesian Velocity Automatic with ValueComponents > OptionInitial Conditions > Cartesian Velocity 0 [m s^-1]Components > UInitial Conditions > Cartesian Velocity 0 [m s^-1]Components > VInitial Conditions > Cartesian Velocity 0 [m s^-1]Components > WInitial Conditions > Static Pressure > Relative 0 [Pa]PressureInitial Conditions > Temperature > Temperature22 [C]Initial Conditions > Turbulence Kinetic Energy >(Selected)Fractional IntensityInitial Conditions > Turbulence Eddy Dissipation(Selected)Initial Conditions > Turbulence Eddy Dissipation(Selected)> Eddy Length ScaleInitial Conditions > Turbulence Eddy Dissipation0.25 [m]> Eddy Length Scale > Eddy Len. ScaleInitial Conditions > Radiation Intensity >(Selected)Blackbody TemperatureInitial Conditions > Radiation Intensity >22 [C]Blackbody Temperature > Blackbody Temp. 3. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settingsTab Setting ValueBasic SettingsTransient Scheme > Option Second Order BackwardEulerConvergence Control > Max. Coeff. Loops 3 3. Click OK.Setting Output Control Transient results files will be set up to record transient values of a chosen set of variables. Monitor points will be created to show the on/off status of the air conditioner, the temperature at the inlet, the temperature at the outlet, and the temperature at a prescribed thermometer location.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 293Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.305. Tutorial 17: Air Conditioning Simulation: Defining a Simulation in ANSYS CFX-Pre1. Click Output Control.2. Click Trn Results.3. Create a new Transient Results item by clicking Add New Itemand accept the the default name.4. Apply the following settings to Transient Results 1Setting ValueOptionSelected VariablesOutput Variables List Pressure, Radiation Intensity, Temperature,VelocityOutput Variables Operators(Selected)Output Variables Operators > Output Var.All*OperatorsOutput Frequency > Option Time IntervalOutput Frequency > Time IntervaltStep *.This causes the gradients of the selected variables to be written to the transient files, along with other information.5. Apply the following settingsTab SettingValueMonitor Monitor Options(Selected)6. Create a new Monitor Points and Expressions item named Temp at Inlet.7. Apply the following settings to Temp at InletSetting ValueOptionExpressionExpression ValueTIn8. Create a new Monitor Points and Expressions item named Thermometer.9. Apply the following settings to ThermometerSetting ValueOutput Variable ListTemperatureCartesian Coordinates 2.95, 1.5, 1.2510. Create a new Monitor Points and Expressions item named Temp at VentOut.11. Apply the following settings to Temp at VentOutSetting ValueOptionExpressionExpression ValueTVentOutPage 294 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.306. Tutorial 17: Air Conditioning Simulation: Obtaining a Solution using ANSYS CFX-Solver Manager 12. Create a new Monitor Points and Expressions item named ACOnStatus. 13. Apply the following settings to ACOnStatusSetting ValueOptionExpressionExpression ValueACOn 14. Click OK.Writing the Solver (.def) File 1. Click Write Solver File . 2. Apply the following settings:Setting ValueFile name HVAC.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at yourdiscretion.Obtaining a Solution using ANSYS CFX-Solver Manager When ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, obtain a solution to the CFD problem by following the instructions below. 1. Click Start Run. 2. When the User Points tab appears, click it to view the value of the temperature atVentOut as the solution progresses. 3. Click Yes to post-process the results when the completion message appears at the endof the run. 4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-Post The temperature of air in the house is distributed in both space and time. While the transient behavior of the temperature field can easily be shown with an animation, it is not easy to visualize a complicated 3D distribution. In order to show the key features of the temperature field, graphic objects will be produced on strategically-placed locators; Plane locators will be used to show contour plots of temperature, while Isosurfaces will be used sparingly to show the general shape of thermal plumes.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 295Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.307. Tutorial 17: Air Conditioning Simulation: Viewing the Results in ANSYS CFX-PostCreating Graphics ObjectsPlane locators will be placed vertically through the vents and horizontally above the floor.Plane Locators1. Load the res file (HVAC_001.res) if you did not elect to load the results directly from the ANSYS CFX-Solver Manager.2. Right-click a blank area in the viewer, select Predefined Camera > Isometric View (Z up).3. Create a ZX-Plane named Plane 1 with Y=1.5 [m]. Color it by Temperature using a user specified range from 19 [C] to 23 [C], and clear Lighting.4. Create an XY Plane named Plane 2 with Z=0.35 [m]. Color it using the same settings as for the first plane, and clear Lighting.Isosurface1. Click Timestep Selector .LocatorThe Timestep Selector appears.2. Double-click the value (12s) in the Timestep Selector. The Timestep is set to 12s so that the cold plume is visible.3. Create an isosurface named Cold Plume which is a surface of Temperature=19 [C]. Use conservative values for Temperature.4. Color the isosurface by Temperature and use the same range as for the planes. Although the color of the isosurface will not show variation (by definition), it will be consistent with the other graphic objects.5. On the Render tab for the isosurface, set Transparency to 0.5, and clear Lighting.6. Click Apply.Note: The isosurface will not be visible in some timesteps, but you will be able to see it whenplaying the animation (a step carried out later).Adjusting the The legend title should not name the locator of any particular object since all objects areLegendcolored by the same variable and use the same range.1. In the tree view, double-click Default Legend View 1.2. In the Definition tab, change Title Mode to Variable. This will remove the locator name from the legend.3. Click the Appearance tab, then:a. Change Precision to 2, Fixed.b. Change Text Height to 0.03.4. Click Apply.A label will be used to show the simulation time and the temperature of the thermometerwhich controls the thermostat. This will be especially useful for the animation which iscreated later in this tutorial.Page 296 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.308. Tutorial 17: Air Conditioning Simulation: Viewing the Results in ANSYS CFX-Post Before creating the label, you will need to support the expression for TSensor by creating a point called Thermometer at the location of the sensor thermometer. This point will replace the monitor point called Thermometer which was used during the solver run, but no longer exists. Note: The actual thermometer data generated during the run was stored in the results file, but is not easily accessible, and cannot currently be used in an auto-annotation label.Creating a Point 1. From the main menu, select Insert > Location > Point.for the2. Set Name to Thermometer.Thermometer 3. Set Point to (2.95,1.5,1.25). 4. Click Apply. Now the expression TSensor will once again measure temperature at the prescribed location.Creating the 1. Click Text .Text Label 2. Accept the default name and click OK. 3. Set Text String to Time Elapsed 4. Select Embed Auto Annotation.The full text string should now be Time Elapsed: . The represents thelocation where the auto annotation will be substituted. 5. Set Type to Time Value.This will show the amount of simulated time that has passed in the simulation. 6. Click More.This adds a second line of text to the text object. 7. Set Text String to Sensor Temperature: 8. Select Embed Auto Annotation. 9. Set Type to Expression. 10. Set Expression to TSensor. 11. Click the Appearance tab, change Height to 0.03, then click Apply. Ensure the visibility check box next to Text 1 is selected. A label appears at the top of the figure. The large font is used so that the text will be clearly visible in the animation which will be produced in the next section.Creating an Animation 1. Ensure that the view is set to Isometric View (Z up). 2. Click Timestep Selector .The Timestep Selector appears. 3. Double-click the first time value (0 s) in the Timestep Selector. 4. Click Animationfound in the toolbar.The Animation dialog box appears. 5. In the Animation dialog box:ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 297Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.309. Tutorial 17: Air Conditioning Simulation: Viewing the Results in ANSYS CFX-Posta. Click Newto create KeyframeNo1.b. Highlight KeyframeNo1, change # of Frames to 200, then press while in the # of Frames box.Tip: Be sure to press and confirm that the new number appears in the list beforecontinuing. This will place 200 intermediate frames between the first and (yet to be created) second key frames, for a total of 202 frames. This will produce an animation lasting about 8.8 s since the frame rate will be 24 frames per second. Since there are 76 unique frames, each frame will be shown at least once.6. Load the last time value (225 s) using the Timestep Selector dialog box.7. In the Animation dialog box:a. Click Newto create KeyframeNo2. The # of Frames parameter has no effect for the last keyframe, so leave it at the default value.b. Click More Animation Optionsto expand the Animation dialog box.c. Select Save MPEG.d. Specify a file name for the MPEG file.e. Click the Options button.f. Change MPEG Size to 720 x 480 (or a similar resolution).g. Click the Advanced tab, and note the Quality setting. If your MPEG player does not play the MPEG, you can try using the Low or Custom quality settings.h. Click OK.i. Click To Beginning to rewind the active key frame to KeyframeNo1.j. Click Save animation stateand save the animation to a file. This will enable you to quickly restore the animation in case you want to make changes. Animations are not restored by loading ordinary state files (those with the .cst extension).8. Click Play the animation.9. If prompted to overwrite an existing movie, click Overwrite. The animation plays and builds an .mpg file.10. When you have finished, quit ANSYS CFX-Post.Further Steps 1. This tutorial uses an aggressive value for the flow rate of air, a coarse mesh, and the timesteps are too large for a satisfactory analysis. Running this tutorial with a finer mesh,a flow rate of air that is closer to 5 changes of air per hour (0.03 m3 s-1), and smallertimesteps will produce more accurate results.2. Running the simulation for a longer total time period will allow you to see more on/off cycles of the thermostat.Page 298 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.310. Tutorial 18:Combustion and Radiation in aCan CombustorIntroduction This tutorial includes: • Tutorial 18 Features (p. 300) • Overview of the Problem to Solve (p. 301) • Using Eddy Dissipation and P1 Models (p. 301) • Defining a Simulation in ANSYS CFX-Pre (p. 302) • Obtaining a Solution using ANSYS CFX-Solver Manager (p. 307) • Viewing the Results in ANSYS CFX-Post (p. 308) • Laminar Flamelet and Discrete Transfer Models (p. 311) • Further Postprocessing (p. 316) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 302). Sample files referenced by this tutorial include: • CombustorMesh.gtm • CombustorEDM.pre • CombustorFlamelet.pre • CombustorEDM.cfxANSYS CFX TutorialsPage 299ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.311. Tutorial 18: Combustion and Radiation in a Can Combustor: Tutorial 18 FeaturesTutorial 18 FeaturesThis tutorial addresses the following features of ANSYS CFX. Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid TypeReacting Mixture Domain Type Single Domain Turbulence Modelk-Epsilon Heat Transfer Thermal Energy Combustion Radiation Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Wall: No-Slip Wall: Adiabatic Wall: Thin Surface TimestepPhysical Time Scale ANSYS CFX-PostPlots Outline Plot (Wireframe) Sampling Plane Slice Plane Vector Other Changing the Color Range Color map Legend Quantitative CalculationIn this tutorial you will learn about:• Creating thin surfaces for the inlet vanes.• Using a Reacting Mixture.• Using the Eddy Dissipation Combustion Model.• Using the Flamelet Model.• Changing the Combustion model in a simulation.• Using the P1 Radiation Model in ANSYS CFX-Pre.• Using the Discrete Transfer Radiation Model in ANSYS CFX-Pre.• Using the NOx model in ANSYS CFX-Pre.• Changing object color maps in ANSYS CFX-Post to prepare a greyscale image.Page 300 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.312. Tutorial 18: Combustion and Radiation in a Can Combustor: Overview of the Problem to SolveOverview of the Problem to Solve The can combustor is a feature of the gas turbine engine. Arranged around a central annulus, can combustors are designed to minimize emissions, burn very efficiently and keep wall temperatures as low as possible. This tutorial is designed to give a qualitative impression of the flow and temperature distributions. The basic geometry is shown below with a section of the outer wall cut away. The Outlet has a surface area of 150 cm2. There are six side air inlets, each with a surface area of 2 cm2.There are six small fuelinlets, each with asurface area of 0.14 cm2.Main air inlet. The inletis guided by vanes togive the air a swirlingvelocity component.Total surface area is57 cm2.Using Eddy Dissipation and P1 Models This tutorial demonstrates two different combustion and radiation model combinations. The first uses the Eddy Dissipation Combustion model with the P1 Radiation model; the NOx model is also included. The second uses the Laminar Flamelet model with the Discrete Transfer Radiation model. If you wish to use the Flamelet Combustion model and Discrete Transfer Radiation model, see Laminar Flamelet and Discrete Transfer Models (p. 311), otherwise continue from this point.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 301Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.313. Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-PreDefining a Simulation in ANSYS CFX-PreYou will define a domain that includes a variable composition mixture. These mixtures areused to model combusting and reacting flows in ANSYS CFX.Playing a Session FileIf you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulationautomatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre,then run the session file: CombustorEDM.pre. After you have played the session file asdescribed in earlier tutorials under Playing the Session File and Starting ANSYS CFX-SolverManager (p. 87), proceed to Obtaining a Solution using ANSYS CFX-Solver Manager (p. 307).Creating a New Simulation1. Start ANSYS CFX-Pre.2. Select File > New Simulation.3. Select General and click OK.4. Select File > Save Simulation As.5. Under File name, type CombustorEDM.6. Click Save.Importing the Mesh1. Right-click Mesh and select Import Mesh.2. Apply the following settingSetting ValueFile name CombustorMesh.gtm3. Click Open.Creating a Reacting MixtureTo allow combustion modeling, you must create a variable composition mixture.To create the 1. Create a new material named Methane Air Mixture.variable2. Apply the following settingscompositionmixtureTabSetting ValueBasic Settings OptionReacting Mixture Material GroupGas Phase Combustion Reactions ListMethane Air WD1 NO PDF*Page 302 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.314. Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-PreTab Setting ValueMixture Mixture Properties(Selected)PropertiesMixture Properties > Radiation Properties > (Selected)†Refractive IndexMixture Properties > Radiation Properties > (Selected)Absorption CoefficientMixture Properties > Radiation Properties > (Selected)Scattering Coefficient *.The Methane Air WD1 NO PDF reaction specifies complete combustion of the fuel into its products in a single-step reaction. The formation of NO is also modeled and occurs in an additional reaction step. Click to display the Reactions List dialog box, then click Import Library Data and select the appropriate reaction to import. †.Setting the radiation properties explicitly will significantly shorten the solution time since the ANSYS CFX-Solver will not have to calculate radiation mixture properties. 3. Click OK.Creating the Domain 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settingsTab SettingValueGeneral Basic Settings > Locations B152, B153, B154,OptionsB155, B156Basic Settings > Fluids List Methane Air MixtureDomain Models > Pressure > Reference Pressure1 [atm]*Fluid ModelsHeat Transfer > Option Thermal EnergyReaction or Combustion > OptionEddy DissipationReaction or Combustion > Eddy Dissipation Model(Selected)Coefficient BReaction or Combustion > Eddy Dissipation Model0.5†Coefficient B > EDM Coeff. BThermal Radiation Model > Option P1Component Details > N2 (Selected)Component Details > N2 > OptionConstraint *.It is important to set a realistic reference pressure in this tutorial because the components of Methane Air Mixture are ideal gases. †.This includes a simple model for partial premixing effects by turning on the Product Limiter. When it is selected, non-zero initial values are required for the products. The products limiter is not recommended for multi-step eddy dissipation reactions, and so is set for this single step reaction only. 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 303Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.315. Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-PreCreating the Boundary ConditionsFuel Inlet1. Create a new boundary condition named fuelin.Boundary2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation fuelinBoundary DetailsMass and Momentum > Normal Speed 40 [m s^-1]Heat Transfer > Static Temperature 300 [K]Component DetailsCH4Component Details > CH4 > Mass Fraction13. Click OK.Bottom Air InletTwo separate boundary conditions will be applied for the incoming air. The first is at theBoundarybase of the can combustor. The can combustor employs vanes downstream of the fuel inletto give the incoming air a swirling velocity.1. Create a new boundary condition named airin.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation airinBoundary DetailsMass and Momentum > Normal Speed 10 [m s^-1]Heat Transfer > Static Temperature 300 [K]Component DetailsO2Component Details > O2 > Mass Fraction 0.232* *.The remaining mass fraction at the inlet will be made up from the constraint component, N2.3. Click OK.Side Air InletThe secondary air inlets are located on the side of the vessel and introduce extra air to aidBoundarycombustion.1. Create a new boundary condition named secairin.2. Apply the following settingsTab SettingValueBasic SettingsBoundary TypeInletLocation secairinPage 304 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.316. Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-PreTab Setting ValueBoundary DetailsMass and Momentum > OptionNormal SpeedMass and Momentum > Normal Speed6 [m s^-1]Heat Transfer > OptionStatic TemperatureHeat Transfer > Static Temperature300 [K]Component Details O2Component Details > O2 > Mass Fraction0.232* *.The remaining mass fraction at the inlet will be made up from the constraint component, N2. 3. Click OK.Outlet 1. Create a new boundary condition named out.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type OutletLocationoutBoundary DetailsMass and Momentum > OptionAverage Static PressureMass and Momentum > Relative Pressure 0 [Pa] 3. Click OK.Vanes Boundary The vanes above the main air inlet are to be modeled as thin surfaces. To create a vane as a thin surface in ANSYS CFX-Pre, you must specify a wall boundary condition on each side of the vanes. The Create Thin Surface Partner feature in ANSYS CFX-Pre will automatically match the other side of a thin surface if you pick just a single side. You will first create a new region which contains one side of each of the eight vanes, then use the Create Thin Surface Partner feature to match the other side. 1. Create a new composite region named Vane Surfaces. 2. Apply the following settingsTabSetting ValueBasic Settings Dimension (Filter)2D* Region List F129.152, F132.152, F136.152, F138.152, F141.152, F145.152, F147.152, F150.152 *.This will filter out the 3D regions, leaving only 2D regions 3. Click OK. 4. Create a new boundary condition named vanes. 5. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 305Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.317. Tutorial 18: Combustion and Radiation in a Can Combustor: Defining a Simulation in ANSYS CFX-PreTab SettingValueBasic SettingsBoundary TypeWallLocation Vane SurfacesCreate Thin Surface Partner(Selected)* *.This feature will attempt to match all primitives specified in the location list to create a thin surface boundary condition.6. Click OK.Default WallThe default boundary condition for any undefined surface in ANSYS CFX-Pre is a no-slip,Boundarysmooth, adiabatic wall.• For radiation purposes, the wall is assumed to be a perfectly absorbing and emittingsurface (emissivity = 1).• The wall is non-catalytic, i.e., it does not take part in the reaction.Since this tutorial serves as a basic model, heat transfer through the wall is neglected. As aresult, no further boundary conditions need to be defined.Setting Initial Values1. Click Global Initialization .2. Apply the following settingsTabSettingValueGlobal Initial Conditions > Cartesian Velocity Components > Automatic with ValueSettings Option Initial Conditions > Cartesian Velocity Components > U 0 [m s^-1] Initial Conditions > Cartesian Velocity Components > V 0 [m s^-1] Initial Conditions > Cartesian Velocity Components > W 5 [m s^-1] Initial Conditions > Turbulence Eddy Dissipation (Selected) Initial Conditions > Turbulence Eddy Dissipation > Automatic Option Initial Conditions > Component Details O2 Initial Conditions > Component Details > O2> OptionAutomatic with Value Initial Conditions > Component Details > O2 > Mass 0.232* Fraction Initial Conditions > Component Details CO2 Initial Conditions > Component Details > CO2 > OptionAutomatic with Value Initial Conditions > Component Details > CO2 > Mass0.01 Fraction Initial Conditions > Component Details H2O Initial Conditions > Component Details> H2O > Option Automatic with Value Initial Conditions > Component Details > H2O > Mass0.01 FractionPage 306 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.318. Tutorial 18: Combustion and Radiation in a Can Combustor: Obtaining a Solution using ANSYS CFX-Solver Manager *.The initial conditions assume the domain consists mainly of air and the fraction of oxygen in air is 0.232. A small mass fraction of reaction products (CO2 and H2O) is needed for the EDM model to initiate combustion. 3. Click OK.Setting Solver Control 1. Click Solver Control . 2. Apply the following settingsTabSetting ValueBasic Settings Convergence Control > Max. Iterations 100 Convergence Control > Fluid Timescale Control > Physical Timescale Timescale Control Convergence Control > Fluid Timescale Control > 0.025 [s] Physical Timescale 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settings:Setting ValueFile name CombustorEDM.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file.Obtaining a Solution using ANSYS CFX-Solver Manager The ANSYS CFX-Solver Manager will be launched after ANSYS CFX-Pre saves the definition file. You will be able to obtain a solution to the CFD problem by following the instructions below. Note: If a fine mesh is used for a formal quantitative analysis of the flow in the combustor, the solution time will be significantly longer than for the coarse mesh. You can run the simulation in parallel to reduce the solution time. For details, see Obtaining a Solution in Parallel (p. 116). 1. Ensure Define Run is displayed.Definition File should be set to CombustorEDM.def.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 307Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.319. Tutorial 18: Combustion and Radiation in a Can Combustor: Viewing the Results in ANSYS CFX-Post2. Click Start Run. ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long time depending on your system. Eventually a dialog box is displayed stating that the run has finished.3. Click Yes to post-process the results.4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Viewing the Results in ANSYS CFX-PostWhen ANSYS CFX-Post opens, experiment with the Edge Angle setting for the Wireframeobject and the various rotation and zoom features in order to place the geometry in asensible position. A setting of about 8.25 should result in a detailed enough geometry forthis exercise.Temperature Within the Domain1. Create a new plane named Plane 1.2. Apply the following settingsTab SettingValueGeometryDefinition > MethodZX PlaneColor Mode VariableMode > VariableTemperature3. Click Apply.The large area of high temperature through most of the vessel is due to forced convection.Note: Later in this tutorial (see Laminar Flamelet and Discrete Transfer Models (p. 311)), theLaminar Flamelet combustion model will be used to simulate the combustion again,resulting in an even higher concentration of high temperatures throughout the combustor.The NO Concentration in the CombustorIn the next step you will color Plane 1 by the mass fraction of NO to view the distributionof NO within the domain. The NO concentration is highest in the high temperature regionclose to the outlet of the domain.1. Modify the plane named Plane 1.2. Apply the following settingsTab SettingValueColor Mode > VariableNO.Mass Fraction3. Click Apply.Page 308 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.320. Tutorial 18: Combustion and Radiation in a Can Combustor: Viewing the Results in ANSYS CFX-PostPrinting a Greyscale Graphic Here you will change the color map (for Plane 1) to a greyscale map. The result will be a plot with different levels of grey representing different mass fractions of NO. This technique is especially useful for printing, to a black and white printer, any image that contains a color map. Conversion to greyscale by conventional means (i.e., using graphics software, or letting the printer do the conversion) will generally cause color legends to change to a non-linear distribution of levels of grey. 1. Modify the plane named Plane 1. 2. Apply the following settingsTab Setting ValueColor Color Map Inverse Greyscale 3. Click Apply.Calculating NO Mass Fraction at the Outlet The emission of pollutants into the atmosphere is always a design consideration for combustion applications. In the next step, you will calculate the mass fraction of NO in the outlet stream. 1. Select Tools > Function Calculator or click the Tools tab and select FunctionCalculator. 2. Apply the following settingsTab Setting ValueFunctionFunctionmassFlowAveCalculatorLocationoutVariableNO.Mass Fraction 3. Click Calculate. A small amount of NO is released from the outlet of the combustor. This amount is lower than can normally be expected, and is mainly due to the coarse mesh and the short residence times in the combustor.Viewing Flow Field To investigate the reasons behind the efficiency of the combustion process, you will next look at the velocity vectors to show the flow field. You may notice a small recirculation in the center of the combustor. Running the problem with a finer mesh would show this region to be a larger recirculation zone. The coarseness of the mesh in this tutorial means that this region of flow is not accurately resolved. 1. Select the Outline tab. 2. Under User Locations and Plots, clear Plane 1.Plane 1 is no longer visible.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 309Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.321. Tutorial 18: Combustion and Radiation in a Can Combustor: Viewing the Results in ANSYS CFX-Post3. Create a new vector named Vector 1.4. Apply the following settingsTab SettingValueGeometryDefinition > Locations Plane 1SymbolSymbol Size25. Click Apply.6. Create a new plane named Plane 2.7. Apply the following settingsTab SettingValueGeometryDefinition > MethodXY PlaneDefinition > Z 0.03Plane Bounds > TypeRectangularPlane Bounds > X Size0.5 [m]Plane Bounds > Y Size0.5 [m]Plane Type > Sample(Selected)Plane Type > X Samples 30Plane Type > Y Samples 30RenderDraw Faces (Cleared)8. Click Apply.9. Modify Vector 1.10. Apply the following settingTab SettingValueGeometryDefinition > Locations Plane 211. Click Apply.To view the swirling velocity field, right-click in the viewer and select Predefined Camera >View Towards -Z.You may also want to turn off the wireframe visibility. In the region near the fuel and airinlets, the swirl component of momentum (theta direction) results in increased mixing withthe surrounding fluid and a higher residence time in this region. As a result, more fuel isburned.Viewing RadiationTry examining the distribution of Incident Radiation and Radiation Intensitythroughout the domain.When you are finished, quit ANSYS CFX-Post.Page 310 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.322. Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer ModelsLaminar Flamelet and Discrete Transfer Models In this second part of the tutorial, you will start with the simulation from the first part of the tutorial and modify it to use the Laminar Flamelet combustion and Discrete Transfer radiation models. Running the simulation a second time will demonstrate the differences in the combustion models, including the variance in carbon dioxide distribution, which is shown below.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: CombustorFlamelet.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining a Solution (p. 314).Creating a New Simulation 1. If you have not completed the first part of this tutorial, or otherwise do not have thesimulation file from the first part, start ANSYS CFX-Pre and then play the session fileCombustorEDM.pre. The simulation file CombustorEDM.cfx will be created. 2. Start ANSYS CFX-Pre (unless it is already running). 3. Select File > Open Simulation. 4. Load the simulation named CombustorEDM.cfx.The simulation from the first part of this tutorial is loaded. 5. Select File > Save Simulation As.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 311Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.323. Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer Models6. Save the simulation as CombustorFlamelet.cfx.This creates a separate simulation file which will be modified to use the LaminarFlamelet and Discrete Transfer models.Modifying the Reacting MixtureA flamelet library will be used to create the variable composition mixture.1. Expand Materials and open Methane Air Mixture for editing.2. Apply the following settingsTabSetting ValueBasic Settings Reactions ListMethane Air FLL STP and NO PDF* *.Click to display the Reactions List dialog box, then click Import Library Data and select the appropriate reaction to import.3. Click OK.Note: Some physics validation messages appear after this reaction is selected. In thissituation, the messages can be safely ignored as the physics will be corrected once thedomains and boundary conditions are modified.Modifying the Domain1. Double-click the Default Domain.2. Apply the following settingsTabSetting ValueFluid Models Reaction or Combustion > Option PDF Flamelet Thermal Radiation Model > OptionDiscrete Transfer Component Details N2 Component Details > N2 > Option Constraint Component Details NO Component Details > NO > Option Transport Equation Component Details (All other components)* Component Details > (All other components)Automatic > Option *.Select these one at a time and check each of them.3. Click OK.Modifying the Boundary ConditionsFuel Inlet1. Modify the boundary condition named fuelin.Boundary2. Apply the following settingsPage 312 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.324. Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer ModelsTab Setting ValueBoundary DetailsMixture > OptionFuelComponent Details NOComponent Details > NO > Option Mass FractionComponent Details > NO > Mass Fraction0 3. Click OK.Bottom Air Inlet 1. Modify the boundary condition named airin.Boundary 2. Apply the following settingsTab Setting ValueBoundary DetailsMixture > OptionOxidiserComponent Details NOComponent Details > NO > Option Mass FractionComponent Details > NO > Mass Fraction0 3. Click OK.Side Air Inlet 1. Modify the boundary condition named secairin.Boundary 2. Apply the following settingsTab Setting ValueBoundary DetailsMixture > OptionOxidiserComponent Details NOComponent Details > NO > Option Mass FractionComponent Details > NO > Mass Fraction0 3. Click OK.Setting Initial Values 1. Click Global Initialization . 2. Apply the following settingsTabSetting ValueGlobal Initial Conditions > Component DetailsNOSettings Initial Conditions > Component Details > NO > OptionAutomatic with Value Initial Conditions > Component Details > NO > Mass0 Fraction 3. Click OK.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 313Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.325. Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer ModelsSetting Solver ControlTo reduce the amount of CPU time required for solving the radiation equations, you canselect to solve them only every 10 iterations.1. Click Solver Control.2. Apply the following settingsTab SettingValueAdvancedDynamic Model Control > Global Dynamic Model Control (Selected)OptionsThermal Radiation Control(Selected)Thermal Radiation Control > Iteration Interval (Selected)Thermal Radiation Control > Iteration Interval > Iteration 10Interval3. Click OK.Writing the Solver (.def) File1. Click Write Solver File .2. Apply the following settings:Setting ValueFile name CombustorFlamelet.defQuit CFX–Pre* (Selected) *.If using ANSYS CFX-Pre in Standalone Mode.3. Ensure Start Solver Manager is selected and click Save.4. If using Standalone Mode, quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining a SolutionWhen ANSYS CFX-Pre has shut down and the ANSYS CFX-Solver Manager has started, obtaina solution to the CFD problem by following the instructions below.1. Ensure Define Run is displayed. Definition File should be set to CombustorFlamelet.def.2. Click Start Run. ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long time depending on your system. Eventually a dialog box is displayed.3. Click Yes to post-process the results.4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.Page 314 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.326. Tutorial 18: Combustion and Radiation in a Can Combustor: Laminar Flamelet and Discrete Transfer ModelsViewing the ResultsViewing1. Create a new plane named Plane 1.Temperaturewithin the Note: If ANSYS CFX-Post was not closed since CombustorEDM.def was processed, allDomain meshes and locators from that session will be retained and updated when the CombustorFlamelet.def is opened. In this way Plane 1 does not need to be remade. 2. Apply the following settingsTab Setting ValueGeometryDefinition > Method ZX PlaneDefinition > Y0Color ModeVariableMode > Variable Temperature 3. Click Apply.Viewing the NO 1. Modify the plane named Plane 1.concentration in 2. Apply the following settingsthe CombustorTab Setting ValueColor Mode > Variable NO.Mass Fraction 3. Click Apply.Calculating NO The next calculation shows the amount of NO at the outlet.Concentration 1. Select Tools > Function Calculator or click the Tools tab and select FunctionCalculator. 2. Apply the following settingsTab Setting ValueFunctionFunctionmassFlowAveCalculatorLocationoutVariableNO.Mass Fraction 3. Click Calculate.Viewing CO The next plot will show the concentration of CO (carbon monoxide), which is a by-productConcentrationof incomplete combustion and is poisonous in significant concentrations. As you will see, the highest values are very close to the fuel inlet and in the regions of highest temperature. 1. Modify the plane named Plane 1. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 315Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.327. Tutorial 18: Combustion and Radiation in a Can Combustor: Further PostprocessingTab SettingValueColor Mode > VariableCO.Mass FractionRangeLocal3. Click Apply.Calculating CO In the next step, you will calculate the mass fraction of CO in the outlet stream.Mass Fraction at 1. Select Tools > Function Calculator or click the Tools tab and select Functionthe OutletCalculator.2. Apply the following settingsTab SettingValueFunctionFunction massFlowAveCalculatorLocation outVariable CO.Mass Fraction3. Click Calculate.There is approximately 0.4% CO by mass in the outlet stream.Further Postprocessing1. Try putting some plots of your choice into the Viewer. You can plot the concentration of other species and compare values to those found for the Eddy Dissipation model.2. Examine the distribution of Incident Radiation and Radiation Intensity throughout the domain.3. Load one combustion model, then load the other using the Add to current results option in the Load Results File dialog box. You can compare both models in the viewer at once, in terms of mass fractions of various materials, as well as total temperature and other relevant measurements.Page 316 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.328. Tutorial 19:Cavitation Around a HydrofoilIntroduction This tutorial includes: • Tutorial 19 Features (p. 318) • Overview of the Problem to Solve (p. 319) • Creating an Initial Simulation (p. 319) • Obtaining an Initial Solution using ANSYS CFX-Solver Manager (p. 323) • Viewing the Results of the Initial Simulation (p. 324) • Preparing a Simulation with Cavitation (p. 326) • Obtaining a Cavitation Solution using ANSYS CFX-Solver Manager (p. 328) • Viewing the Results of the Cavitation Simulation (p. 328) If this is the first tutorial you are working with it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 319). Sample files referenced by this tutorial include: • HydrofoilExperimentalCp.csv • HydrofoilGrid.def • HydrofoilIni.pre • Hydrofoil.pre • HydrofoilIni_001.resANSYS CFX TutorialsPage 317ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.329. Tutorial 19: Cavitation Around a Hydrofoil: Tutorial 19 FeaturesTutorial 19 Features This tutorial addresses the following features of ANSYS CFX.Component Feature DetailsANSYS CFX-Pre User Mode General ModeSimulation Type Steady StateFluid TypeGeneral FluidDomain Type Single DomainTurbulence Modelk-EpsilonHeat Transfer IsothermalMultiphaseBoundary Conditions Inlet (Subsonic)Outlet (Subsonic)Symmetry PlaneWall: No-SlipWall: Free-SlipTimestepPhysical Time ScaleANSYS CFX-Solver ManagerRestartANSYS CFX-PostPlots ContourLine LocatorPolylineSlice PlaneStreamlineVectorOther Chart CreationData ExportPrintingTitle/TextVariable Details View In this tutorial you will learn about: • Modeling flow with cavitation. • Using vector reduction in ANSYS CFX-Post to clarify a vector plot with many arrows. • Importing and exporting data along a polyline. • Plotting computed and experimental results.Page 318ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.330. Tutorial 19: Cavitation Around a Hydrofoil: Overview of the Problem to SolveOverview of the Problem to Solve This example demonstrates cavitation in the flow of water around a hydrofoil. A two-dimensional solution is obtained by modeling a thin slice of the hydrofoil and using two symmetry boundary conditions.cavitation zone 16.91 m s^-1 In this tutorial, an initial solution with no cavitation is generated to provide an accurate initial guess for a full cavitation solution, which is generated afterwards.Creating an Initial Simulation This section describes the step-by-step definition of the flow physics in ANSYS CFX-Pre.Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the session file: HydrofoilIni.pre. After you have played the session file as described in earlier tutorials under Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87), proceed to Obtaining an Initial Solution using ANSYS CFX-Solver Manager (p. 323).Defining the Simulation 1. Start ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Select General and click OK. 4. Select File > Save Simulation As. 5. Under File name, type HydrofoilIni. 6. Click Save.Importing the Mesh 1. Right-click Mesh and select Import Mesh. The Import Mesh dialog box appears. 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 319Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.331. Tutorial 19: Cavitation Around a Hydrofoil: Creating an Initial Simulation Setting Value File type CFX-Solver (*.def, *.ref, *.trn, *.bak) File name HydrofoilGrid.def 3. Click Open. 4. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z.Loading Materials Since this tutorial uses Water Vapour at 25 C and Water at 25 C you need to load these materials. 1. In the Outline tree view, right-click Materials and select Import Library Data.The Select Library Data to Import dialog box is displayed. 2. Expand Water Data. 3. Select both Water Vapour at 25 C and Water at 25 C by holding whenselecting. 4. Click OK.Creating the Domain The fluid domain used for this simulation contains liquid water and water vapour. The volume fractions are initially set so that the domain is filled entirely with liquid. 1. Right click Simulation in the Outline tree view and ensure that Automatic DefaultDomain is selected. A domain named Default Domain should now appear under theSimulation branch. 2. Double click Default Domain and apply the following settings TabSettingValue GeneralBasic Settings > Fluids List*Water at 25 C, Water Options Vapour at 25 CDomain Models > Pressure > Reference Pressure0 [atm] Fluid Models Multiphase Options > Homogeneous Model (Selected)Heat Transfer > Option IsothermalHeat Transfer > Fluid Temperature300 [K]Turbulence > Optionk-Epsilon*.These two fluids have consistent reference enthalpies. 3. Click OK.Creating the Boundary Conditions The simulation requires inlet, outlet, wall and symmetry plane boundary conditions. The regions for these boundary conditions were imported with the grid file.Page 320ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.332. Tutorial 19: Cavitation Around a Hydrofoil: Creating an Initial SimulationInlet Boundary 1. Create a new boundary condition named Inlet. 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type InletLocationINBoundary DetailsMass and Momentum > Normal Speed16.91 [m s^-1]Turbulence > Option Intensity and Length ScaleTurbulence > Value0.03Turbulence > Eddy Len. Scale0.0076 [m]Fluid ValuesBoundary Conditions Water at 25 CBoundary Conditions > Water at 25 C>1Volume Fraction > Volume FractionBoundary Conditions Water Vapour at 25 CBoundary Conditions > Water Vapour at 25 C > 0Volume Fraction > Volume Fraction 3. Click OK.Outlet 1. Create a new boundary condition named Outlet.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type OutletLocationOUTBoundary DetailsMass and Momentum > OptionStatic PressureMass and Momentum > Relative Pressure 51957 [Pa] 3. Click OK.Free Slip Wall 1. Create a new boundary condition named SlipWalls.Boundary 2. Apply the following settingsTab Setting ValueBasic SettingsBoundary Type WallLocationBOT, TOPBoundary DetailsWall Influence on Flow > Option Free Slip 3. Click OK.Symmetry Plane 1. Create a new boundary condition named Sym1.Boundaries 2. Apply the following settingsANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 321Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.333. Tutorial 19: Cavitation Around a Hydrofoil: Creating an Initial Simulation Tab SettingValue Basic SettingsBoundary TypeSymmetry Location SYM1 3. Click OK. 1. Create a new boundary condition named Sym2. 2. Apply the following settings Tab SettingValue Basic SettingsBoundary TypeSymmetry Location SYM2 3. Click OK.Setting Initial Values 1. Click Global Initialization . 2. Apply the following settings TabSetting Value Global Initial Conditions > Cartesian Velocity Components >Automatic with Value Settings OptionInitial Conditions > Cartesian Velocity Components > U16.91 [m s^-1]Initial Conditions > Cartesian Velocity Components > V0 [m s^-1]Initial Conditions > Cartesian Velocity Components > W0 [m s^-1]Initial Conditions > Turbulence Eddy Dissipation(Selected) FluidFluid Specific Initialization Water Settings at 25 CFluid Specific Initialization > Water at 25 C (Selected)Fluid Specific Initialization > Water at 25 C > Initial Automatic with ValueConditions > Volume Fraction > OptionFluid Specific Initialization > Water at 25 C > Initial 1Conditions > Volume Fraction > Volume FractionFluid Specific Initialization Water Vapour at 25 CFluid Specific Initialization > Water Vapour at 25 C(Selected)Fluid Specific Initialization > Water Vapour at 25 C > Initial Automatic with ValueConditions > Volume Fraction > OptionFluid Specific Initialization > Water Vapour at 25 C > Initial 0Conditions > Volume Fraction > Volume Fraction 3. Click OK.Page 322ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.334. Tutorial 19: Cavitation Around a Hydrofoil: Obtaining an Initial Solution using ANSYS CFX-Solver ManagerSetting Solver Control 1. Click Solver Control . 2. Apply the following settingsTab SettingValueBasic SettingsConvergence Control > Max. Iterations35Convergence Control > Fluid TimescalePhysical TimescaleControl > Timescale ControlConvergence Control > Fluid Timescale0.01 [s]Control > Physical Timescale Note: For the Convergence Criteria, an RMS value of at least 1e-05 is usually required for adequate convergence, but the default value is sufficient for demonstration purposes. 3. Click OK.Writing the Solver (.def) File 1. Click Write Solver File. 2. Apply the following settingsSetting ValueFile name HydrofoilIni.defQuit CFX–Pre *(Selected) *.If using ANSYS CFX-Pre in Standalone Mode. 3. Ensure Start Solver Manager is selected and click Save. 4. Quit ANSYS CFX-Pre, saving the simulation (.cfx) file at your discretion.Obtaining an Initial Solution using ANSYS CFX-Solver Manager While the calculations proceed, you can see residual output for various equations in both the text area and the plot area. Use the tabs to switch between different plots (e.g., Momentum and Mass, Turbulence Quantities, etc.) in the plot area. You can view residual plots for the fluid and solid domains separately by editing the workspace properties. 1. Ensure that the Define Run dialog box is displayed. 2. Click Start Run.ANSYS CFX-Solver runs and attempts to obtain a solution. This can take a long timedepending on your system. Eventually a dialog box is displayed. 3. Click Yes to post-process the results. 4. If using Standalone Mode, quit ANSYS CFX-Solver Manager.ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Page 323Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.335. Tutorial 19: Cavitation Around a Hydrofoil: Viewing the Results of the Initial SimulationViewing the Results of the Initial Simulation The following topics will be discussed: • Plotting Pressure Distribution Data (p. 324) • Exporting Pressure Distribution Data (p. 325) • Saving the Post-Processing State (p. 326)Plotting Pressure Distribution Data In this section, you will create a plot of the pressure coefficient distribution around the hydrofoil. The data will then be exported to a file for later comparison with data from the cavitating flow case, which will be run later in this tutorial. 1. Right-click a blank area in the viewer and select Predefined Camera > View Towards-Z. 2. Insert a new plane named Slice. 3. Apply the following settings Tab SettingValue GeometryDefinition > MethodXY Plane Definition > Z 5e-5 [m] RenderDraw Faces (Cleared) 4. Click Apply. 5. Create a new polyline named Foil by selecting Insert > Location > Polyline from themain menu. 6. Apply the following settings Tab SettingValue GeometryMethod Boundary Intersection Boundary ListDefault Domain Default Intersect With Slice 7. Click Apply.Zoom in on the center of the hydrofoil (near the cavity) to confirm the polyline wrapsaround the hydrofoil. 8. Create a new variable named Pressure Coefficient. 9. Apply the following settings Setting Value Expression(Pressure-51957[Pa])/(0.5*996.2[kg m^-3]*16.91[m s^-1]^2) 10. Click Apply. 11. Create a new variable named Chord. 12. Apply the following settingsPage 324ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved.Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.336. Tutorial 19: Cavitation Around a Hydrofoil: Viewing the Results of the Initial SimulationSetting ValueExpression(X-minVal(X)@Foil)/(maxVal(X)@Foil-minVal(X)@Foil) This creates a normalized chord, measured in the X direction, ranging from 0 at the leading edge to 1 at the trailing edge of the hydrofoil. 13. Click Apply. Note: Although the variables that were just created are only needed at points along the polyline, they exist throughout the domain. Now that the variables Chord and Pressure Coefficient exist, they can be associated with the previously defined polyline (the locator) to form a chart line. This chart line will be added to the chart object, which is created next. 1. Select Insert > Chart from the main menu. 2. Set the name to Pressure Coefficient Distribution. 3. Apply the following settingsTab SettingValueChart TitlePressure Coefficient DistributionLabels > Use Data For Axis Label (Cleared)Labels > X AxisNormalized Chord PositionLabels > Y AxisPressure CoefficientChart Line 1Line NameSolver CpLocation FoilX Axis > VariableChordY Axis > VariablePressure CoefficientAxesX Axis > Determine Ranges Automatically(Cleared)X Axis > Min 0X Axis > Max 1Y Axis > Determine Ranges Automatically(Cleared)Y Axis > Min -0.5Y Axis > Max 0.4Y Axis > Invert Axis (Selected) 4. Click Apply. 5. The chart appears on the Chart Viewer tab.Exporting Pressure Distribution Data You will now export the chord and pressure coefficient data along the polyline. This data will be imported and used in a chart later in this tutorial for comparison with the results for when cavitation is present. 1. Select File > Export. The Export dialog box appears 2. Apply the following settingsANSYS CFX Tutorials. ANSY